# Loss of mass

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

 April 17, 2003, 16:27 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

 April 18, 2003, 03:09 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?

 April 18, 2003, 04:14 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.

 April 19, 2003, 11:26 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

 April 21, 2003, 16:53 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

 April 23, 2003, 09:33 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

 April 23, 2003, 10:24 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

 April 23, 2003, 13:00 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

 April 23, 2003, 15:59 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Attesz CFX 7 January 5, 2013 04:32 kit STAR-CD 3 April 13, 2010 11:34 saii CFX 2 September 18, 2009 08:07 jinwon park Main CFD Forum 13 May 22, 2008 09:29 asarum FLUENT 1 March 2, 2005 05:49

All times are GMT -4. The time now is 09:52.