CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Spalart-Allmaras model (http://www.cfd-online.com/Forums/cfx/85588-spalart-allmaras-model.html)

siw March 2, 2011 03:39

Spalart-Allmaras model
 
Hi,

having successfully run a series of compressible aerodynamics simulations using the SST model I chose to try the Spalart-Allmaras model as a comparison on the same mesh (y+=1).

Firstly, I'm using v12.1 so the S-A model is a beta feature, but it still seems to be at v13. Also there's no mention of it in the help guide.

In the first iteration I got this message repeatedly:

The non-dimensional near wall temperature (T+) has be clipped
for calculation of Wall Heat Transfer Coefficient.


Boundary Condition : Fuselage
T+ clip value = 1.0000E-10


if this situation persists and you are using the High Speed Model,consider enabling mach number based blending between low speed and high speed wall functions. you can do so by specifying a Mach number threshold as follows:


EXPERT PARAMETERS:
highspeed wf mach threshold = 0.1 # default=0.0 (off)
END

Firstly, i assume that when is says "High Speed Model" it means using Air Ideal Gas and Total Energy which is for compressible flows (which I am using).

Also, I cannot find this parameter in the Expert Parameters, so how can I set it?

Thanks

lukaswang March 2, 2011 06:36

i have the same problem

joey2007 March 3, 2011 14:35

There is something basic wrong. Did you test your setup with one of standard turbulence models?

siw March 3, 2011 16:10

Like I put in my first post I did use the k-omega SST model first and it was all okay.

siw March 17, 2011 03:15

Here's the fix to this problem I had as it may help others.

It works if the turbulent wall function = scalable

Originally, I set it to default thinking that CFX would select the most appropriate, but that caused the error. Noting about this model is mentioned in the CFX guides.

joey2007 March 18, 2011 15:50

well, it is beta.


Thanks for providing the solution for the others.

Mazze[ITA] May 11, 2011 02:31

Unfortunately Ansys doesn't provide documentation for beta features... I tried lo launch a Spalart-Allmaras run in CFX13, using scalable turb wall function, but it returns me an error:

| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Missing boundary condition closure attribute for variable TKE_FL-1 |

| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine CAL_VAR_BCS |

Did you have the same problem?

Far May 11, 2011 05:07

I have used the SA model in CFX 12. for compressor rotor successfully. I used the default, automatic and scalable option. I think scalable option is not good or it need more working by CFX. As far the other options are concerned they are essentially same and giving the same results. I tried the yplus from 1 to 60 and results up to yplus 10 are exactly same and deviates little at yplus 60

Mazze[ITA] May 11, 2011 05:23

I think CFX13 lost the automatic option... Did you use default values for the other options ?

Far May 11, 2011 09:13

automatic option is not available in pre even in CFX 12. for this you have to edit the def file from solver

Mazze[ITA] May 11, 2011 09:16

Quote:

Originally Posted by Far (Post 307200)
automatic option is not available in pre even in CFX 12. for this you have to edit the def file from solver

thank you for this suggestion!

Far May 11, 2011 09:16

yes default values, if you need i can send you my all cfx files

Far May 11, 2011 09:20

as i guess these terms have following meaning

default = low re formulation originally suggest by spalart allmars

automatic = hybrid wall treatment by blending the log layer and linear profile for yplus between yplus 6 (or 2 i am not sure) and yplus 30

scalable = assumes first cell point is at y plus = 11.06 even mesh is designed to be yplus = 1

Mazze[ITA] May 11, 2011 09:23

Quote:

Originally Posted by Far (Post 307203)
yes default values, if you need i can send you my all cfx files

First I'll make a try, in case of unsuccess I'll contact you. Thanks again!

Far May 11, 2011 09:24

http://www.cfd-online.com/Forums/cfx...machinery.html


check results of different yplus with automatic wall treatment and comparison with scalable and experimental data at above link (2nd attachment )

Far May 18, 2011 06:36

Any update on results? did you contact the support team for the SA model documentation

Mazze[ITA] May 18, 2011 06:58

both default and scalable treatment return me the same error... I don't know what to do and I think beta features are not supported.

Far May 18, 2011 19:07

There must not be any error with beta SA model. I have used it very successfully

Mazze[ITA] May 19, 2011 02:17

What about boundary condition ? Did you setup the valure for \tilde{\nu}?

Far May 19, 2011 02:40

No. Just pick the SA and run it with scalable, automatic and default. No difficulty at all


All times are GMT -4. The time now is 12:49.