CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   Predicition of pseudo shock with Spalart-allmaras (

DaveM September 11, 2007 11:35

Predicition of pseudo shock with Spalart-allmaras
Hi, i'm working with a 2d simulation of a supersonic diffuser using Spalart-Allmaras+2nd order upwind. My mach number is 2. The results didn't show clearly the pseudoshock pattern. This pattern results from interaction of shockwaves and turbulent boundary layer . I want to know if i could do something for improve the prediction with Spalart-Allmaras model or if you can help me with other ideas.

Joe September 11, 2007 12:31

Re: Predicition of pseudo shock with Spalart-allma
Grid resolution? yplus?

DaveM September 11, 2007 13:13

Re: Predicition of pseudo shock with Spalart-allma
313986 quadrilateral cells. Y+ between 2.5 and 1 boundary conditions=pressure inlet and pressure outlet. Symmetry boundary and wall boundary.

Joe September 11, 2007 16:00

Re: Predicition of pseudo shock with Spalart-allma
Adapt on pressure gradient to sharpen grid at shocks.

DaveM September 11, 2007 18:56

Re: Predicition of pseudo shock with Spalart-allma
ok,thank you. i'm going to try it.

raj September 12, 2007 01:43

Re: Predicition of pseudo shock with Spalart-allma

from my experience i saw that pres. inlet and outlet are not the best of BC's you can use for supersonic flow, instead spread out your grid all over and apply pr.farfield conditions, they will definitely help the purpose, but must go for unsteady analysis.

sridhar September 12, 2007 11:54

Re: Predicition of pseudo shock with Spalart-allma
Hi I am also working on somewhat a similar case, but mine is s supersonic combustor ..with inlet at mach 2...I am getting a sort of psudo shocks..I was initially unaware of any thing of that sort then I had to go through some literature...but my solution is not able to 'conserve mass' and the pattern after the psudo shock is fully turbulent.. can u suggest some good literature where I can know more about Pseudo shocks and flow after it.. Thanks N regards

Andy R September 13, 2007 12:42

Re: Predicition of pseudo shock with Spalart-allma
I do supersonic inlets, diffusers and combustors in Fluent all the time. I also use GASP when the customer allows, but...

I find that if you have reasonable grid resolution Fluent will do a reasonable job.

I use Double Precision, density based (coupled), implicit solver.

I generally use AUSM for the flux type.

I use standard K-e (old faithful!)with y+ between 10 and 100.

I generally find the if the shocks / expansion waves begin to dominate the flow, I need to use second order to conserve mass.

I use pressure far-field for my "inlet".

I use a pressure-outlet for my "outlet"

Have you applied enough backpressure to actually cause a shock and/or made sure your isolator is long enough for the BL growth to cause the shock/seperation?

Fluent should be able to get an OK answer if you can use enough grid. For higher fidelity you may need to look at a code like GASP or VULCAN, as they are purpose build for such problems.

Good Luck - Andy R

sridhar September 13, 2007 13:27

Re: Predicition of pseudo shock with Spalart-allma
Andy do u have any idea about my case .. S/s Combustion.. if yes then please help.. my mass flow is not getting conserved..


DaveM September 13, 2007 17:42

Re: Predicition of pseudo shock with Spalart-allma
Thanks Andy R. All these ideas have showed me other ways that i didn't have contemplated!!.

Dany Rincon September 14, 2007 01:39

Similar problem
Hi Well, i have contacted DaveM , we both have a similar problem, but my case is with the supersonic diffuser for a SUPERSONIC WIND TUNNEL simulation.

The solution always diverges (almost 100 tries). I am modeling with S-A viscous model, density based (coupled) solver implicit, Inlet boundary with Pressure inlet, outlet boundary with Pressure outlet. Second order upwind.

I only get a solution with the pressure inlet (only with it), no pressure inlet nor operating pressure allowed because diverges.

If anybody can help me , i really would appreciate it.

Andy R September 14, 2007 15:55

Re: Similar problem
Danny, Generally I find you can't start any compressible solutions in fluent at second order, you need to get some resonable flow field with first order and then switch over. I normally use GASP for Wind Tunnel nozzles, but if I had to do that in fluent I would start (and this will seem a bit strange) with a fixed inlet mass flow. You should be able to determine from first principles the choked flow to use. It will try and match total temp and adjust the static P at the inlet to get the required mass flow. Once the sonic throat is established, you should be able to switch over.

NOTE: I havent done this my self but a few colleuges have had some success with this approach in fluent.

Also I find fluent needs a starting CFL number of less than 0.5 sometimes as low as 0.1. I have had some succes using the FMG initialization, which was somewhat supprising to me but a good suprise ;-)

You may want to try that to get a good initial flow feild. Getting things "started" can be tricky in the real world and so it is in the virtual one.

Good Luck - Andy R

Dany Rincon September 14, 2007 16:40

Re: Similar problem
Thank you for your response Andy

Well, i am not very expert in Fluent, so i don't understand well some things you suggest me.

First, is CFL number the Courant number? Second, What is FMG initialization?

It would be excellent contact you directly, to show you some of the results so you could suggest me any solution more precisely.

Again, thank you very much for your suggestions, i will be waiting for your response.

All times are GMT -4. The time now is 18:29.