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

GradU in Post

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 4, 2003, 04:59
Default GradU in Post
  #1
sch
Guest
 
Posts: n/a
Hi All. In CFX-post I would like to plot velocity gradients (for example Velocity u.Gradient X). I noticed that these quantities are not always available in the list of the variable selector. They are only if the solve was done using high differentiation scheme for the advection term. Why? how to have this quantities in any case?

Thank you
  Reply With Quote

Old   September 4, 2003, 10:07
Default Re: GradU in Post
  #2
Robin
Guest
 
Posts: n/a
The gradient terms are required to calculate the second order Numerical Advection Correction (NAC). If you use the 1st Order Upwind Differencing Scheme (UDS) (which you really shouldn't use...), these terms are not required and are not calculated.

The general second order advection scheme is calculated by adding the UDS value and NAC value, with the second order correction multiplied by a blend factor, Beta:

Advected Quantity = UDS + Beta*NAC

Therefore a Beta value of 1 is fully second order whereas a Beta value of 0 is only first order. If you really want UDS results but with the gradient terms, use the specified blend factor scheme instead and set the blend factor to zero.

(If you run the High Resolution scheme, Beta is calculated locally to keep the solution bounded.)

Best regards, Robin
  Reply With Quote

Old   September 4, 2003, 12:00
Default Re: GradU in Post
  #3
sch
Guest
 
Posts: n/a
Robin Thank you for your help. I tried my run with BETA=0, but I still can not get the velocity gradients. I used 1st order scheme only for tests purposes.

Regards sch
  Reply With Quote

Old   September 4, 2003, 13:39
Default Re: GradU in Post
  #4
Robin
Guest
 
Posts: n/a
Hey, you're right! Looks like the solver attempts to save on memory (and time) and doesn't calculate momentum gradients when the blend factor is zero. It should work if you set the blend factor to a very small value, .001 for instance.

Regards, Robin
  Reply With Quote

Old   September 4, 2003, 17:23
Default Re: GradU in Post
  #5
Pascale Fonteijn
Guest
 
Posts: n/a
Hi Robin,

I am trying to solve a case at very low pressures (1-1000 Pa) and very high speeds (Mach >2) with the High-Resolution scheme. When I monitor the ranges during the run I see that under certain conditions the absolute pressure becomes neagtive although density remains positive: it becomes very low (1e-10). The solver can continue with this unrealistic set of data for around 15 iterations but finally blows up.

Now, you say the solution is bounded (no unrealistic over- and undershoots) because the Beta value is calculated locally. This does seems to apply for density but not for pressure, or am I wrong? Can you shed a light? How can I prevent the diverging behavior?

Thanks, Pascale.
  Reply With Quote

Old   September 4, 2003, 17:56
Default Re: GradU in Post
  #6
Robin
Guest
 
Posts: n/a
Hi Pascale,

The converged solution will be bounded, but an unconverged solution may not. There are many reasons this may be happening to you; initial guess, timestep, boundary conditions, mesh quality. Since it is problem specific, I suggest contacting support for help.

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
NO model vs post processing in coal combustion,CFX sakalido CFX 1 April 15, 2011 15:07
Export from post gives different result between v11 and v12 bennn CFX 2 February 10, 2011 06:38
post processing for KIVA dirga Main CFD Forum 5 April 23, 2009 11:58
post data starcd_learner CD-adapco 0 February 1, 2006 12:24
Post Processing in FEM Abhijit Tilak Main CFD Forum 0 April 26, 2004 12:59


All times are GMT -4. The time now is 09:30.