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

Flow rate imbalance

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 10, 2010, 17:18
Default Flow rate imbalance
  #1
New Member
 
Join Date: Jun 2010
Posts: 20
Rep Power: 8
serezhkin is on a distinguished road
Hi all,

I am running a steady state calculation where incompressible flow goes from one plenum to the other through several openings in the wall.

I specify the velocity on the inlet such that the flow rate is a certain number (465CFM). The outlet is a pressure boundary.

The problem is, when I go to CFX-Post and calculate massFlow()@Each Opening surface and add them up together, the flow rate through the openings does not match the inlet flow and is in fact much lower (392CFM).

Any ideas on why this is happening are much appreciated.
serezhkin is offline   Reply With Quote

Old   December 11, 2010, 06:14
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,545
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
If your simulation is steady state then you have not adequately converged.
ghorrocks is offline   Reply With Quote

Old   December 12, 2010, 00:56
Default
  #3
New Member
 
Join Date: Jun 2010
Posts: 20
Rep Power: 8
serezhkin is on a distinguished road
It is steady state, and it has converged down to 5E-5 or so on all velocity residuals.
As far as I understand, the mass flow rate imbalance should be down to round-off error within the first 20-30 iterations (I ran 800) for steady-state.
I thought that maybe I am just not calculating the flow rate correctly.

Is there a situation where the result of call to massFlow() is open to interpretation?
serezhkin is offline   Reply With Quote

Old   December 12, 2010, 05:54
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,545
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Global balances are different things to residuals. You can have a simulation with very low residuals but the global balances are still miles off. Anyone who has done CHT simulations will have seen this. In this case you need to specify convergence on residuals AND imbalances. Residuals alone is not sufficient. This is discussed int he documentation.

How are you calculating the mass flows?

Quote:
the mass flow rate imbalance should be down to round-off error within the first 20-30 iterations
Rubbish. A well behaved simulation may have converged in 20-30 iterations but to converge to round off will take a lot longer than that. And if you ran 800 iterations then I suspect your simulation is not well optimised yet so even that may not be enough. And there are plenty of more complex cases when you need thousands of iterations for a steady state run to converge.
ghorrocks is offline   Reply With Quote

Old   December 13, 2010, 14:16
Default
  #5
New Member
 
Join Date: Jun 2010
Posts: 20
Rep Power: 8
serezhkin is on a distinguished road
I am calculating the flow rates using the massFlow() function on the opening surfaces where there is a 1:1 connection between mesh blocks. I am also monitoring the flow rates in solver, and there's less than 0.2% variation over the last 100 iterations or so.

By the way, the only reason I ran 800 iterations is to see if it will make a difference in the mass flow imbalance. The run is converged within 150 iterations.
serezhkin is offline   Reply With Quote

Old   December 13, 2010, 17:33
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,545
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
What do the imbalances at the end of the output file report?
ghorrocks is offline   Reply With Quote

Old   December 15, 2010, 19:34
Default
  #7
New Member
 
Join Date: Jun 2010
Posts: 20
Rep Power: 8
serezhkin is on a distinguished road
All right, I figured it out, so I'll post here in case someone runs into a similar problem.

First of all, my thanks to ghorrocks for his help with the problem.

It looks like Ansys only checks the boundaries of the domain to make sure the flow rate balance is observed. Because all my mesh regions were in same domain, the flow balance between mesh regions was not enforced.

As soon as I split the domain into several domains (with GGI interfaces), CFX realized that there's a flow imbalance and fixed it.

Thus, on the boundary of interest (between mesh regions) the flow rate went up to what it should be (as specified on the inlet BC).
serezhkin 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
Mass Flow Rate Error jallison FLUENT 1 May 16, 2011 16:22
Mass Flow Rate student87 CFX 4 January 2, 2010 05:45
Can circum-avg-axial give flow rate? Amit FLUENT 0 January 10, 2007 12:20
negative global mass flow rate Gimli FLUENT 0 April 21, 2006 07:17
mass flow inlet Denis Tschumperle FLUENT 7 August 9, 2000 02:19


All times are GMT -4. The time now is 22:28.