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

Loss of mass

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 17, 2003, 16:27
Default Loss of mass
  #1
Pascale Fonteijn
Guest
 
Posts: n/a
Hi all,

I am performing CFX 5.5.1-simulations on a chamber with one inlet (pressure boundary) and two outlets (both pressure boundaries). During the simulation the average pressure in the chamber is decreasing ...., keeps on decreasing ...., the outlets are biulding walls for 100% ...., only mass enters through the inlet ..., and still the overall pressure is decreasing. I am loosing mass.... Where does it go? Any explanation?

The inflow through the inlet goes over a restriction where Mach=1, so it can be seen as a sort of mass flow boundary. The mach number in the chamber runs up to 4.

Any help is appreciated, Pascale
  Reply With Quote

Old   April 18, 2003, 03:09
Default Re: Loss of mass
  #2
Holidays
Guest
 
Posts: n/a
What is the initial pressure field? What are the values used at the three inlet/outlets?
  Reply With Quote

Old   April 18, 2003, 04:14
Default Re: Loss of mass
  #3
Pascale Fonteijn
Guest
 
Posts: n/a
The initial pressure is 1000 Pa which is the reference pressure. At the inlet and outlets the relative static pressure is set to 0 Pa. After redistribution of the gas, the pressure near the inlet should drop to around -800 Pa (200 Pa absolute pressure). Near the outlets the pressure should increase to around 1000 Pa (2000 Pa absolute pressure).

Thanks for responding, Pacale.
  Reply With Quote

Old   April 19, 2003, 11:26
Default Re: Loss of mass
  #4
cfddoctor
Guest
 
Posts: n/a
Hi Pascale,

The problem seems to be the initial guess. Try restarting the run with a Local timescale factor of 2 or below, and slowly wean the solution by increasing this factor and finally with a physical timescale. Hope this helps

cfddoctor
  Reply With Quote

Old   April 21, 2003, 16:53
Default Re: Loss of mass
  #5
Robin
Guest
 
Posts: n/a
Hi Pascale,

Am I missing something? You have specified the same pressure for the inlet and the outlet (zero relative), but you eventually expect ther pressure near the inlet to drop to 200 [Pa] and near the outlet to increase to 2000 [Pa]?

Regards, Robin
  Reply With Quote

Old   April 23, 2003, 09:33
Default Re: Loss of mass
  #6
Pascale Fonteijn
Guest
 
Posts: n/a
Hi Robin,

It is some kind of rotating piece of equipment. Low pressure in the centre, high pressure at the far ends.

Pascale
  Reply With Quote

Old   April 23, 2003, 10:24
Default Re: Loss of mass
  #7
Robin
Guest
 
Posts: n/a
Perhaps you could be more specific about the pressures. Did you specify a total pressure at your inlet or a static pressure? As for the pressures you expect to see, are these total or static.

Also, If you expect to see a pressure rise across the system, why is this not reflected in your boundary conditions?

Robin
  Reply With Quote

Old   April 23, 2003, 13:00
Default Re: Loss of mass
  #8
Pascale Fonteijn
Guest
 
Posts: n/a
Hi Robin and cfddoctor,

The pressures specified are static pressures. The inflow and outflows go over restrictions. All restrictions have a high inlet pressure and a low outlet pressure. Mach = 1 is supposed to apply for all.

Of course, in the domain the pressure cannot rise spontaneously from inlet to outlet. However, i cannot elaborate on the physical process...

I will continue with the local time scales factors. Is there a way to let it rise automatically?

Pascale

  Reply With Quote

Old   April 23, 2003, 15:59
Default Re: Loss of mass
  #9
Robin
Guest
 
Posts: n/a
Hi Pascale,

I don't recommend going to a local timestep factor. I think the problem has more to do with your boundary conditions.

A pressure specified inlet is not recommended as it does not define the momentum fully. I recommend specifying the total pressure at your inlet. This should give you much better behavior.

If it is a rotating problem, you timestep should be ~1/Omega, where Omega is the rotation rate in radians per second. You may want to start with a smaller value, but I do not recommend going smaller than .01/Omega. A good timestep to start would be .1/Omega.

You initial guess should also be reasonable. A rough estimate of velocity, pointing in the right direction would be good. A uniform pressure which is lowe than your inlet pressure and higher than you outlet pressure will help things move in the right direction.

Lastly, if you want to update the timestep during the run you will have to wait for 5.6. With 5.6 you can specify the timestep as an expression of iteration number (or time if it is a transient simulation). You can also update the timestep manually during the run using the new Dynamic Update feature (which also allows you to modify boundary conditions and other things).

Good luck. If you are still having trouble, contact technical support. You have some funky setup by the sound of it and support staff will be able to help you out a lot more if they can look at the problem.

Best regards, Robin
  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
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
Star-CD transient simulation, problem of loss of mass kit STAR-CD 3 April 13, 2010 11:34
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
Mass loss! So what? jinwon park Main CFD Forum 13 May 22, 2008 09:29
Help! mass loss in close natural convection asarum FLUENT 1 March 2, 2005 05:49


All times are GMT -4. The time now is 22:13.