Flow rate imbalance

serezhkin · December 10, 2010, 16:18

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.

ghorrocks · December 11, 2010, 05:14

If your simulation is steady state then you have not adequately converged.

serezhkin · December 11, 2010, 23:56

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?

ghorrocks · December 12, 2010, 04:54

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.

serezhkin · December 13, 2010, 13:16

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.

ghorrocks · December 13, 2010, 16:33

What do the imbalances at the end of the output file report?

serezhkin · December 15, 2010, 18:34

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).

December 10, 2010, 16:18	Flow rate imbalance	#1
serezhkin New Member Join Date: Jun 2010 Posts: 20 Rep Power: 15	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.

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 04:45
Can circum-avg-axial give flow rate?	Amit	FLUENT	0	January 10, 2007 11:20
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

December 11, 2010, 05:14		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	If your simulation is steady state then you have not adequately converged.

December 11, 2010, 23:56		#3
serezhkin New Member Join Date: Jun 2010 Posts: 20 Rep Power: 15	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?

December 13, 2010, 13:16		#5
serezhkin New Member Join Date: Jun 2010 Posts: 20 Rep Power: 15	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.

December 13, 2010, 16:33		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	What do the imbalances at the end of the output file report?

December 15, 2010, 18:34		#7
serezhkin New Member Join Date: Jun 2010 Posts: 20 Rep Power: 15	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).