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

Pressure losses

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 26, 2002, 10:35
Default Pressure losses
  #1
René
Guest
 
Posts: n/a
Hi there,

I'm currently trying to simulate airflow into an air intake, using CFX 5.5, but I have problems with the pressure results I get. I started doing simulations on a bellmouth inlet on which I have extensive experimental data. I find that the pressure losses (both static and total) are predicted way too high with the CFX simulations. The losses are over predicted by anything from two to five times as much. I have tried the k-e and SST turbulence models with progressively finer meshes and boundary inflation, but the answers still remain the same. The boundary conditions are defined as Openings (with the static pressure defined) around the control volume and a single mass flow outlet. Did anyone have similar problems before and, more importantly, does anyone have a solution as to what I can do to improve the CFD results? Any comments or suggestions are welcome.

René
  Reply With Quote

Old   March 27, 2002, 01:04
Default Re: Pressure losses
  #2
Robin
Guest
 
Posts: n/a
Hi René,

I recommend setting your inlet boundary condition to "Total Pressure", this is the most sensible for such an inlet. If you were to look at the total pressure distribution at your (static pressure) inlet, you would see some variation. This would be physically incorrect, since it is the total pressure which should be constant in the far field.

Also, what advection scheme are you using?

Robin
  Reply With Quote

Old   March 27, 2002, 04:00
Default Re: Pressure losses
  #3
Neale
Guest
 
Posts: n/a
What sort of convergence levels were you attaining and what do your flow balances look like? The default is 1.0e-4 RMS, you might have to go down to 1.0e-4 MAX to get better results.

The pressure drop will be strongly dependent on the both the inlet turbulence levels and velocity profiles because these strongly influence the boundary layer growth from the inlet. Are you 100% sure about your inlet boundary condition? I think you might want to try a total pressure inlet instead of a static pressure opening as well.

Also, as Robin mentioned, what advection scheme are you using? Upwind is bad. If you are running incompressible flow use a specified blend factor of 1.0. If your running compressible flow, and your flow has shocks in it somewhere then use the high resolution scheme.

Neale
  Reply With Quote

Old   April 8, 2002, 04:45
Default Re: Pressure losses
  #4
Bart Prast
Guest
 
Posts: n/a
>If you are running incompressible flow use a >specified blend factor of 1.0. If your running >compressible flow, and your flow has shocks in it >somewhere then use the high resolution scheme.

a blend factor a 1.0 is not the same as high resolution?
  Reply With Quote

Old   April 8, 2002, 08:13
Default Re: Pressure losses
  #5
cfd guy
Guest
 
Posts: n/a
Hi,
By the way, what means this blend factor?
I always used to work with classical 1st and 2nd order schemes, the classic ones, 1st order: Upwind, Power Law, Hybrid, WUDS, etc.. 2nd: Higher Upwind, Van Leer, etc... But Blend Factor, I never heard about it. Perhaps I should take a look at the manuals.
Sincerely, cfd guy
  Reply With Quote

Old   April 8, 2002, 10:14
Default Re: Pressure losses
  #6
Varig
Guest
 
Posts: n/a
It a parameter for the NAC scheme in CFX-5 isn't it, to blend between Upwind and NAC?
  Reply With Quote

Old   April 8, 2002, 10:45
Default Re: Pressure losses
  #7
Bart Prast
Guest
 
Posts: n/a
blend factor=linear scaling factor between upwind and second order scheme
  Reply With Quote

Old   April 8, 2002, 19:32
Default Re: Pressure losses
  #8
Robin
Guest
 
Posts: n/a
Hi Bart,

A blend factor of 1 sets the discretization scheme to fully second order.

The High Resolution scheme is a bounded second order scheme. This will result in a beta value (blend factor) of 1 throughout most of your domain, but the solver can locally change the value of beta to ensure that there are no "wiggles" in the solution. These "wiggles" develop when the second order correction terms cause unphysical values where sharp discontinuities occur, such as at a free surface or shock. By changing the value of beta, the solution remains physical and offers a sharper solution (hence High Resolution).

If you are curious what value of beta the solver has used, they are written to the results file for each equation set (Velocity U.beta for instance).

Regards, Robin

  Reply With Quote

Old   April 11, 2002, 08:02
Default Re: Pressure losses
  #9
Bart Prast
Guest
 
Posts: n/a
If this high resolution scheme behaves like a TVD scheme with limiter. At what value of the gradients does this scheme then swith from 2nd to 1st order? I wrote my own TVD code (Euler). What I want to know how a TVD scheme behaves in f.i. the boundary layer (steep gradients in tangential velocity)
  Reply With Quote

Old   April 11, 2002, 16:40
Default Re: Pressure losses
  #10
Robin
Guest
 
Posts: n/a
Hi Bart,

The High Resolution scheme does not just switch from 2nd to 1st order (ie Beta=0 or 1). Rather, it will set Beta to whatever value it takes to keep the results physical (i.e. eliminating overshoots and undershoots). I'm not sure what what exactly occurs in the boundary layer, but if you are curious, you could set up a simulation and look at the beta values near the wall.

Robin
  Reply With Quote

Old   April 12, 2002, 08:33
Default Re: Pressure losses
  #11
cfd guy
Guest
 
Posts: n/a
You said that we can check out these Beta values. So I ask you, these values are in the .res file by default, or must I add any extra expert parameters?


Sincerely, cfd guy
  Reply With Quote

Old   April 12, 2002, 08:55
Default Re: Pressure losses
  #12
Robin
Guest
 
Posts: n/a
They are in there by default. In Post, the pull-down menu of variables gives you a short list of commonly desired variables, click on the [...] button next to it and you will get the full list.

Of course, the beta values are only there if you ran High Resolution.

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
pressure inlet & outlet. help ASAP Plz engahmed Main CFD Forum 0 June 13, 2010 15:34
Help ASAP! pressure inlet & outlet engahmed FLUENT 0 June 13, 2010 15:33
Pressure losses for compressible flows chouki FLUENT 0 November 21, 2008 04:47
Pressure Inlet yields wrong velocities Ben FLUENT 0 November 21, 2004 02:47
pressure losses Olivier Macchion CFX 5 December 13, 2002 05:43


All times are GMT -4. The time now is 17:48.