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

A wall has been placed at outlet

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 28, 2013, 16:30
Default A wall has been placed at outlet
  #1
Member
 
Karthick Selvam
Join Date: Oct 2012
Location: Germany
Posts: 48
Rep Power: 4
selvam2487 is on a distinguished road
Send a message via Skype™ to selvam2487
Dear Friends,

During my LES calculations, I am getting the information that a wall is placed at about 60 % of the outlet region to prevent the fluid flow back into domain. I cannot understand why this is happening. I am attaching a part of my out file and ccl file along with this mail for your information. Kindly have a look at it and let me know the mistake I am making. Thank you.

I am attaching the link for ccl and out file for reference.

https://www.dropbox.com/s/pv7u53f2gefdt35/Files.7z

P.S: Usually during my LES calculations, I will get a value of around 7 to 8 % regions at outlet where wall has been placed. This is the first time I am getting a very high number like this. I am sure I have made some mistake but I cannot understand the nature of this problem and why it happens.

Thank you for your help in advance.

Regards,
Karthick Selvam
selvam2487 is offline   Reply With Quote

Old   October 28, 2013, 17:37
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This is an FAQ: http://www.cfd-online.com/Wiki/Ansys...f_an_OUTLET.22

If it does not seem to be affecting your results then I would ignore it. A sensitivity check between this and an opening (which allows backflow) would be useful.
ghorrocks is offline   Reply With Quote

Old   October 30, 2013, 04:05
Default Wall at outlet
  #3
Member
 
Karthick Selvam
Join Date: Oct 2012
Location: Germany
Posts: 48
Rep Power: 4
selvam2487 is on a distinguished road
Send a message via Skype™ to selvam2487
Dear Glenn,

Thanks for your reply. Yesterday when I was checking my .out file again and I observed that

(i) During some iterations there was a wall placed at 100% of the outlet region in order to avoid the fluid flow back into the domain. My domain length downstream of T junction (the simulation that I am currently doing) is about 20 diameters. All my important measuring points lie within the first 10 diameters downstream of T junction. I have extended the computational domain by further 10 diameters in anticipation of these problems.

(ii) Usually the percentage of wall placed at the outlet for my simulations are in the range of 10-15%. This is the first time that I am getting 100% of wall placed at outlet. Will this affect the parameters in my monitor points region (in the range of 5-8 diameters downstream of T junction)?

Thanks for the reply in advance.

Regards,
Karthick Selvam
selvam2487 is offline   Reply With Quote

Old   October 30, 2013, 06:03
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The trick of extending the outlet downstream does not work so well for LES. In LES you have turbulent eddies which will have parts where the flow is going backwards. This means you will almost always have some backflow somewhere. The amount of backflow will vary and it is possible that occasionally it becomes very high. But 100% backflow is a worry, that suggests you had numerical problems at this point.

Can you use an opening? That can handle backflow with no problems.
ghorrocks is offline   Reply With Quote

Old   October 30, 2013, 09:24
Default Backflow problem
  #5
Member
 
Karthick Selvam
Join Date: Oct 2012
Location: Germany
Posts: 48
Rep Power: 4
selvam2487 is on a distinguished road
Send a message via Skype™ to selvam2487
Dear Glenn,

I tried the same simulation with increased mesh elements and with a lower time step (0.0002 s). Initially it was ok and it showed that wall had been placed at 50-60% of outlet at certain inner co-efficient loops. In general, it is showing that wall had been placed at 20-40 % of outlet. I am interested in knowing your comments about it.

Also, I am now in the process of trying an opening and seeing how it works.

Thank you
Regards,
Karthick Selvam
selvam2487 is offline   Reply With Quote

Old   October 30, 2013, 17:44
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you are doing LES then a finer mesh and time steps will resolve more turbulent eddies and you should get more backflow. This is not surprising.

But if you are doing LES then the choice of mesh size is a critical simulation parameter as you have to get the resolution of the anisotropic turbulent eddies, but leave the isotropic ones unresolved. You cannot just change the mesh size and see what happens with LES - it is a carefully chosen decision and once taken you should not change it.

But yes, you should look at openings.
ghorrocks is offline   Reply With Quote

Old   November 3, 2013, 03:20
Default Wall at outlet
  #7
Member
 
Karthick Selvam
Join Date: Oct 2012
Location: Germany
Posts: 48
Rep Power: 4
selvam2487 is on a distinguished road
Send a message via Skype™ to selvam2487
Dear Glenn,

I was looking at some of the older posts in this forum about the same problem as I have now and found that you had suggested to switch on the conservation target check box in the solver control tab and set it to a default of 0.01. I switched it on and ran the simulation and observed that it works fine now.

- It is now showing that wall is placed at 14 -15 % of the outlet region, which is what I usually encounter in all my LES.

- Does this mean that the simulation works fine now or should I monitor some other parameters?

I am attaching the residual and domain imbalance snapshot taken from CFX solver control for your reference. The portion circled in the picture is the effect of setting the conservation target to 0.01.
Thank you for your help and guidance.

Regards,
Karthick
Attached Images
File Type: jpg Residuals.jpg (52.5 KB, 18 views)
File Type: jpg Domain Imbalance.jpg (52.2 KB, 14 views)
selvam2487 is offline   Reply With Quote

Old   November 3, 2013, 06:03
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Adding imbalances to the convergence criteria just means you are converging tighter. If this changes the result then your previous convergence tolerance was too loose.

You really need to do convergence tolerance sensitivity checks before you start reading too much into your results. And while you are at it, check time step size and mesh size - but as previously mentioned mesh and timestep size is intimately linked to the filtering length/time scales so you have to check your turbulence length/time scales to make sure you are resolving it correctly.
ghorrocks is offline   Reply With Quote

Old   November 3, 2013, 09:57
Default Time step and mesh size
  #9
Member
 
Karthick Selvam
Join Date: Oct 2012
Location: Germany
Posts: 48
Rep Power: 4
selvam2487 is on a distinguished road
Send a message via Skype™ to selvam2487
I use a time step size of 0.0002 s, which keeps the courant number less than 1 for all the iterations. Based on the journal reference posted in the FAQ section, I calculated my average cell size to be around 1.18 mm. Also, the y plus value shown in the CFD post is around 5-6. But I am surely interested in checking the domain imbalance and convergence criteria performance on a much refined mesh.
selvam2487 is offline   Reply With Quote

Old   November 3, 2013, 17:39
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Courant Number has only a low relevance to CFX as it is an implicit solver. You are getting mixed up with explicit solvers where Courant number is critical. Just because Courant number <1 that does not mean you have a time step size independant solution. You need to check.
ghorrocks is offline   Reply With Quote

Old   November 4, 2013, 03:32
Default
  #11
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 522
Rep Power: 11
Lance is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Courant Number has only a low relevance to CFX as it is an implicit solver. You are getting mixed up with explicit solvers where Courant number is critical. Just because Courant number <1 that does not mean you have a time step size independant solution. You need to check.
This is true, but Ansys recommends a Courant number ono the order of 0.5-1 for LES applications to resolve transient details. See the LES timestep considerations in CFX modeling guide.
Lance is offline   Reply With Quote

Old   November 4, 2013, 05:25
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
True. And I suspect in LES adaptive timestepping will constant jiggle the time step up and down with the turbulent fluctuations and that is not a good thing either.
ghorrocks is offline   Reply With Quote

Reply

Tags
les, t junction

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
Inlet and outlet boudary without wall between Janshi CFX 5 February 2, 2012 05:51
A wall has been placed at portion(s) of an OUTLET aero123 CFX 1 November 9, 2011 19:14
solution problem : A wall has been placed at portion(s) of an OUTLET alnabhani CFX 1 August 8, 2010 18:46
Combining BCs: wall - outlet. Boundary layer disappears MartinaF OpenFOAM Running, Solving & CFD 1 July 20, 2009 18:14
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 12:47.