# GradU in Post

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 September 4, 2003, 03:59 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

 September 4, 2003, 09:07 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

 September 4, 2003, 11:00 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

 September 4, 2003, 12:39 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

 September 4, 2003, 16:23 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.

 September 4, 2003, 16:56 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

 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 sakalido CFX 1 April 15, 2011 14:07 bennn CFX 2 February 10, 2011 06:38 dirga Main CFD Forum 5 April 23, 2009 10:58 starcd_learner Siemens 0 February 1, 2006 12:24 Abhijit Tilak Main CFD Forum 0 April 26, 2004 11:59

All times are GMT -4. The time now is 08:39.

 Contact Us - CFD Online - Privacy Statement - Top