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

ANSYS CFX Solver Domain Imbalance

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 15, 2014, 00:37
Default ANSYS CFX Solver Domain Imbalance
  #1
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 5
amodpanthee is on a distinguished road
I am doing CFD analysis of pelton turbine using ANSYS. THe CFX solver shows domain imbalance, attached. My domain consists of a stationary domain and rotary domain. I was looking if anybody could explain the physical meaning of domain imbalance. The value changes from positive value to negative value.
Attached Images
File Type: jpg 111.JPG (78.0 KB, 103 views)
amodpanthee is offline   Reply With Quote

Old   January 15, 2014, 06:53
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,273
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The domain imbalance is simply the sum of that variable over the domain's boundaries. So for mass, it is the the sum of all the inlets plus the outlets (noting that flow into the domain is positive and out is negative). If conservation is achieved this will sum to zero (assuming no mass sources or sinks, or accumulation of mass in the domain). If it does not sum to zero the imbalance gives you the magnitude of the imbalance and it is up to up to determine if that is a problem or not. This is also done for momentum, heat and any other equations you are using.

The imbalances you are showing are pretty large for most applications so most people would not consider your simulation converged. So best run it longer to reduce the imbalances. Even better, add imbalances to the convergence criteria and it will keep running until the imbalances are down to your defined tolerance.
ghorrocks is offline   Reply With Quote

Old   January 15, 2014, 07:22
Default
  #3
Senior Member
 
JuPa's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 312
Rep Power: 7
JuPa is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Even better, add imbalances to the convergence criteria and it will keep running until the imbalances are down to your defined tolerance.
In solver control, select "Consvervation Target" and set it to a small value, say 0.01 or anything of your choice (between 1 and 0).
JuPa is offline   Reply With Quote

Old   February 5, 2015, 17:17
Default
  #4
Member
 
Marcel Jay
Join Date: Jun 2014
Location: Berlin
Posts: 53
Rep Power: 4
marcel_jay is on a distinguished road
Thanks for your hint to judge the conservation yourself. But what do you think on this one:

I have a rotating Domain (x-axis), with a cylindrical opening. My residuals and monitor points seem to converge pretty nicely, but the imbalances seem really high. U-Mom is quite low with 1% imbalance whereas W-Mom and V-Mom are between 9% and 11%.
I would suspect this to be due to the rotation of the opening and the air in and outflow.

Cheers,
Marcel
Attached Images
File Type: jpg domain.jpg (28.7 KB, 36 views)
marcel_jay is offline   Reply With Quote

Old   February 5, 2015, 21:37
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,273
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Possibly. But it does mean that it is highly likely your simulation is not adequately converged. You might be able to fix it by simply running the simulation longer (I presume this is a steady state or frozen rotor simulation).
ghorrocks is offline   Reply With Quote

Old   February 6, 2015, 05:28
Default
  #6
Member
 
Marcel Jay
Join Date: Jun 2014
Location: Berlin
Posts: 53
Rep Power: 4
marcel_jay is on a distinguished road
Thank you for your advice. yes it is steady state, but I already run about 300 iterations with auto timestep. don't really know if thats adequate as I'm not too long in the cfd business.
marcel_jay is offline   Reply With Quote

Old   February 6, 2015, 05:44
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,273
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Then simply run it longer and watch the imbalances in the solver manager. They should by converging to zero - if so then just run it longer for tighter convergence. If they are still bouncing around consult this FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
ghorrocks is offline   Reply With Quote

Old   February 6, 2015, 10:12
Default
  #8
Member
 
Marcel Jay
Join Date: Jun 2014
Location: Berlin
Posts: 53
Rep Power: 4
marcel_jay is on a distinguished road
Thank you, I will try that.
marcel_jay is offline   Reply With Quote

Old   March 8, 2016, 08:18
Default
  #9
Member
 
Marcel Jay
Join Date: Jun 2014
Location: Berlin
Posts: 53
Rep Power: 4
marcel_jay is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
The domain imbalance is simply the sum of that variable over the domain's boundaries. So for mass, it is the the sum of all the inlets plus the outlets (noting that flow into the domain is positive and out is negative).
So far I used the Imbalances a good indicator for my convergence.
What I encountered now is hard for me to grasp. The p-Mass-Flow is fluctuating between 100% and -100%, jumping like square function.
Hence I was asking myself how it is calculated exactly. Since my userpoints indicate good convergence, I didn't think this behaviour shows bad convergence.
marcel_jay is offline   Reply With Quote

Old   March 8, 2016, 18:55
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,273
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
That is why imbalances are not the default convergence option.

Image this: If you have a box with only a single opening, mass conservation tells you that there will be no net mass flow through the opening. But in a numerical simulation there is errors and noise, so there will be a tiny flow caused by numerical noise (let's call the flow rate m). The imbalance calculation is the imbalance divided by the total flow, so that is m/m which is either +1 or -1 depending on the flow direction. And that is why the imbalances flick between 100% and -100%.
ghorrocks 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
FSI simulation in ansys cfx Arash67.m CFX 0 August 11, 2012 07:18
CFX domain comparison Kiat110616 CFX 4 April 3, 2011 22:43
why the solver reject it? Anyone with experience? bearcat CFX 6 April 28, 2008 14:08
Cancel a domain in CFX solver Neser25 CFX 2 February 19, 2007 12:19
ANSYS to acquire CFX Fred CD-adapco 0 February 18, 2003 22:03


All times are GMT -4. The time now is 23:37.