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

How to Monitor Mass flow rate in CFX

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

Like Tree2Likes
  • 1 Post By opaque
  • 1 Post By Robin

Reply
 
LinkBack Thread Tools Display Modes
Old   September 12, 2007, 11:46
Default How to Monitor Mass flow rate in CFX
  #1
Md Hamidur
Guest
 
Posts: n/a
Hi, I am simulting flow over a axial gas turbine blade with 30 stator blade and 60 rotor blade. I want to see convergence of mass flow rate at a perticular point in the domain. I know this could be done from user monitor option. But mass flow rate option is not available. Could anyone please tell me how to do that?
  Reply With Quote

Old   September 12, 2007, 12:23
Default Re: How to Monitor Mass flow rate in CFX
  #2
Robin
Guest
 
Posts: n/a
Hi Hamidur,

Mass Flow cannot be calculated at a point, you need a surface through which to define the mass flow. The residuals tell you the imbalance, but CFX only reports the Maximum (MAX) and Root Mean Square (RMS) residual. I don't think you can output the residual at a point.

What exactly is your concern? If you are concerned about the imbalance of mass, this is calculated as the mass into the domain minus the mass out of the domain and is reported to the monitor file already, you just need to plot it.

Regards, Robin
  Reply With Quote

Old   September 12, 2007, 13:14
Default Re: How to Monitor Mass flow rate in CFX
  #3
Md Hamidur
Guest
 
Posts: n/a
Thanks for your comments. Actually I need to plot Mass flow rate against the iteration. This plot is possible in fluent but I am not sure about CFX.
  Reply With Quote

Old   September 12, 2007, 14:00
Default Re: How to Monitor Mass flow rate in CFX
  #4
opaque
Guest
 
Posts: n/a
Dear Md Hamidur,

You are not being specific on which Mass Flow Rate you want? Do you want the mass flow rate on the inlet, outlet, a 2d region within the domain?

If you know which 2d region you want, you can monitor it by creating a Output Control/Monitor Points. Select the option Expression and type somethin along the lines of

Expression = massflow()@YourInlet

Expression = massflow()@TheOutlet

Expression = massflow()@REGION: some defined region

Hope it helps,

Opaque

amirhnp likes this.
  Reply With Quote

Old   September 13, 2007, 13:59
Default Re: How to Monitor Mass flow rate in CFX
  #5
HekLer
Guest
 
Posts: n/a
This can be done in CFX, just as easy as Fluent.

In addition to opaque's comments, which require you to create a monitor point in CFX Pre, you do not need to do this if you want to monitor the mass flow rate through an existing boundary condition (eg: inlet, outlet, interface boundary, etc..):

- Create a new montior in the solver manager and call it something, say "My Mass Flow Monitor"

- Pick "FLOW" in the tree

- Pick the domain name you want and then the boundary you want

- Monitor the "P-Mass" flow through that boundary

  Reply With Quote

Old   September 13, 2007, 14:25
Default Re: How to Monitor Mass flow rate in CFX
  #6
Hamidur Rahman
Guest
 
Posts: n/a
Thank you guys. I did it succesfully. One more problem that I have been experiencing now and that is "wall has been placed at the outlet boundary". I know that it means there is a reverse flow at the exit of the domain. Is there any way to get rid of this instead of playing with the boundary condition? Thanks to you all
  Reply With Quote

Old   September 14, 2007, 09:08
Default Re: How to Monitor Mass flow rate in CFX
  #7
Dothan
Guest
 
Posts: n/a
Hi, I think the only method is to move the surface where you define the BC, il the problem is well posed.

I belive that wall placed by CFX can help the convergence for the initial iterations but if the convergence is reached with this notice, the solution is totally unphysic.

Remain to understand if this notice disapper, is the final solution affected by the convergence story?

Dothan
  Reply With Quote

Old   September 14, 2007, 10:50
Default Re: How to Monitor Mass flow rate in CFX
  #8
Robin
Guest
 
Posts: n/a
Hi Hamidur,

It depends on what's going on at the outlet. You should try and match the physical conditions as closely as possible. If there is likely to be separation and recirculation near the outlet and this is a region of interest, you should move your outlet further downstream to resolve the necessary flow features. If your outlet is far from the region of interest, you can probably ignore the warning.

Before you modify your geometry, consider trying some of the other options for the outlet mass flow specification. By default the solver will scale the local flow rate at the outlet to allow a natural pressure profile to develop. Other options are to set the mass flow to "Constant Flux" and "Scale Pressure".

Constant Flux will enforce a uniform mass flux across the surface. This is what most codes do at a mass flow outlet, but may be unphysical. It is useful for bleeds or outlets where you just want to pull the mass out and aren't concerned about the profile and is usually more stable.

Scale Pressure requires that you enter a pressure profile (by CEL), which the solver will shift up and down in order to get the appropriate mass flow rate. A very common way to use this is to simply specify a constant value for the pressure profile (any constant value will do), in which case the boundary condition will have a constant static pressure across the face. This is physically realistic if your outlet ejects into a larger domain or plenum.

Regards, Robin
A_Prakash likes this.
  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: calculation v/s computation beguxa FLUENT 4 June 8, 2013 16:17
Compressible Flow in Ansys CFX bcheruk CFX 11 February 26, 2011 19:40
in CFX, how to define a inlet condition of feedback control flow rate ? suihenry CFX 12 May 14, 2009 17:59
mass flow rate error Masood FLUENT 0 May 22, 2005 00:32
Mass Flow Rate Calculation Paul FLUENT 9 March 23, 2002 09:37


All times are GMT -4. The time now is 14:31.