CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   GradU in Post (http://www.cfd-online.com/Forums/cfx/19869-gradu-post.html)

sch September 4, 2003 03:59

GradU in Post
 
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

Robin September 4, 2003 09:07

Re: GradU in Post
 
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

sch September 4, 2003 11:00

Re: GradU in Post
 
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

Robin September 4, 2003 12:39

Re: GradU in Post
 
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

Pascale Fonteijn September 4, 2003 16:23

Re: GradU in Post
 
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.

Robin September 4, 2003 16:56

Re: GradU in Post
 
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


All times are GMT -4. The time now is 17:37.