Shock induced Seperation 1

[Nickul18]

Anybody had any experience of predicting seperation due to a shock. We know it is wrong as our prediction does not line up with our experiment, but are struggling to find a method to correctly predict this phenomenon.

we are using fluent , with standard K-e , 2nd order discretization.

 

[btrueblood]

Is the problem that you are not predicting seperation (i.e. it is really occurring in experiment) or that you are predicting seperation in the model, and not seeing it in experiments?

 

[Nickul18]

we're predicting the seperation prematurely in the model where as in the experiment it does not occur until a reasonable distance downstream.

 

[btrueblood]

Okay. I've had similar problems using the NASA/AF NPARC code. Predicting b.l. seperation is one of the trickiest problems in CFD, and predicting shock-induced seperation is practically black art (or at least it was 5+ years ago). You could surf the NPARC/Wind website to find information/papers regarding shock-induced seperation (see * below). I seem to recall that using a k-omega (see ** below) instead of a k-e formulation helped reduce the size of the seperation bubble near the shock, but didn't move the seperation zone appreciably. The k-e model in general performs poorly in regions of adverse pressure gradients; many "adjustments" have been made by researchers to improve it, with generally lacluster success. The other thing to try is to massively subgrid (or otherwise increase grid density) in the shock/wall zone to give better resolution of pressure gradients across the shock. Finally, an approach that I'd considered and discussed with colleagues, but never tried (lacked the wind tunnel data for the particular problem), was to "turn off" the k-e model upstream of where we thought the seperation would occur, i.e. run a laminar (or even inviscid) model upstream, and only apply k-e model where you believe the seperation zone will begin (essentially you force the model to put the seperation where you want it). That method is what I believe is typically done by those who really want to drive to a low-error solution.

*

http://www.grc.nasa.gov/

http://WWW/wind/valid/transdif/transdif.html

**[Menter, F. R. (1993) "Zonal Two Equation k-? Turbulence Models for Aerodynamic Flows," AIAA Paper 93-2906; Mani, M., Ladd, J. A., Cain, A. B., and Bush, R. H.(1997) "An Assessment of One- and Two-Equation Turbulence Models for Internal and External Flows," AIAA Paper 97-2010]

 

[Nickul18]

cheers , yeah I'm trying the K-w model at the moment but I'm a bit skeptical as to the results.
Certainly adapting the grid will be another area of investigation , but I have 100K cells in the region that contains the shock with a good BL mesh as well, (all hex).
I will check out the validation case as well, thats a very good link I was not aware of that. Bit baffled as to the boundary conditons as the pressure ratio is very much below the critical ratio, but I'm sure it will become clear as I look into it, anyhow the grid file supplied has imported into gambit nicely which is an all time first !

 

[btrueblood]

Nick,

Note that none of the models appears to do a good job of predicting both seperation and/or re-attachment accurately.

Do you have access to the source code for Fluent, so that you could try coding in some of the corrections mentioned in the NPARC/Wind papers? Alternatively, do you have a job in the U.S., for a US company? If so, you can ask for copy of the NPARC and Wind codes. It costs a nominal amount ($50? IIRC) for the distribution/mailing/handling fee, but you get the source code. Which of course, means you need a compiler. The coolest thing about Wind and NPARC are their ability to run on a Beowulf cluster (parallel processing "supercomputer" network, running Linux).

Good luck with your task. Would love to hear if Fluent can do as well or better than Wind at the validation problem.