CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

CFX problems with supersonic inlet condition - Inlet values in CFX-Post are wrong

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 22, 2011, 17:43
Default CFX problems with supersonic inlet condition - Inlet values in CFX-Post are wrong
  #1
New Member
 
Join Date: Jan 2010
Posts: 5
Rep Power: 7
jannnesss is on a distinguished road
Hey!!!!

I am setting up a 2D-simulation in CFX 12.01 with an supersonic inlet and supersonic outlet boundary condition.
I need to simulate the supersonic flow in a 2D-channel with a ramp.
I specified p, T and u at the inlet. The calculation works fine, no errors or something else.

But when I check the results in CFX post (or tecplot) I can see some problems at the inlet. For example: When I use the functionCalculator in post, the static temperature calculated at the inlet is the value I gave CFX as boundary condition (when I calculate it hybrid). But when I calculate the temperature "conservative" the value is not the same I gave CFX as boundary condition.

For those who don't know the calculator in post.
The temperature at the cell face is correct like I said CFX as boundary condition. But when I check the temparature one cell further in the domain (free slip walls for the first cells in the domain) the static temperature is approximately 10 K higher than the value I gave CFX as boundary conditon. The same for the Mach number.

Please help me, because it looks more or less like a bug because the calculation itself works fine and the flowfield is also okay!!! The only thing which is wrong, is that the the "real" inlet condition is wrong because of the effect I described above....

best regards and thanks a lot!!!!!
jannnesss is offline   Reply With Quote

Old   February 22, 2011, 18:16
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,651
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Are you sure your boundary is correct? Usually this sort of effect is the solver establishing equilibrium to account for boundary specification errors.
ghorrocks is offline   Reply With Quote

Old   February 22, 2011, 19:07
Default
  #3
New Member
 
Join Date: Jan 2010
Posts: 5
Rep Power: 7
jannnesss is on a distinguished road
Well, I think everything should be allright.
The Mach number, static temperature and static pressure is given...
I used the NASA-Format from CFX to calculate the corresponding specific heat capacitiy in order to calculate from the Mach number the velocity (u=sqrt(kappa*R*T)*Ma). After one calculation I used for the next one the specific heat capacity calculated from CFX post at the inlet.

The only value which could be incorrect is in my opinion the velocity at the inlet. I forgot to mention above, the same effect as for the temperature occurs for the velocity and pressure.

The temperature increases about 10 K
The pressure increases about 500 Pa
The velocity decreases about 10 m/s

And this gap occurs in the first cell!!!
Maybe it is because of an inaccuracy in the specific heat capacity (-> kappa)
jannnesss is offline   Reply With Quote

Old   February 23, 2011, 10:24
Default
  #4
New Member
 
Join Date: Mar 2009
Posts: 9
Rep Power: 8
CycLone is on a distinguished road
Is the passage expanding? Is the solution converged?

Check the total conditions at both locations. Your total pressure and temperature should be about the same. An increase in static temperature and pressure are consistent with a decrease in velocity. If the total conditions are the same, look for why the velocity is decreasing. An expanding passage would explain this.
CycLone is offline   Reply With Quote

Old   February 23, 2011, 17:00
Default
  #5
Member
 
Join Date: Feb 2010
Location: Australia
Posts: 65
Rep Power: 7
RossFS is on a distinguished road
You will get a significant difference between hybrid and conservative boundaries near a boundary/wall based on the difference in how they are calculated (its a finite volume thing - look them up in xref.pdf provided in the ANSYS installation somewhere).

Also, this thread might be of use as I was modelling a similar flow and encountered a number of problems along the way (still unresolved) including T and P issues like you have mentioned:
Is CFX incapable of modelling a compression ramp in 2D?
RossFS is offline   Reply With Quote

Old   February 25, 2011, 17:24
Default
  #6
New Member
 
Join Date: Jan 2010
Posts: 5
Rep Power: 7
jannnesss is on a distinguished road
Hey guys!!!

thanks for your advice!!!!

Now I know the problem, and it might help you (RossFS) as well.
The problem in my case was the turbulence model. I used the EARSM model, but this was not the problem. The main problem was the CFX option "medium intensity" for the turbulence boundary condition at the inlet.
Because of the high inlet velocity the kinetic turbulent energy was overestimated by CFX. I tried two options, zero gradient and a fixed value for the turbulent kinetic energy & turbulent eddy dissipation. Both worked...

I am not sure if the explenation is correct, but I think the high turbulent kinetic energy (which is a boundary condition) gets his energy from the free stream...maybe something like an energy transfer which looks like an compression (T up, p up, u down)

Thanks for you advice....the best method is definitely to simplify the model!! (new test geometry, laminar, ideal air and so on....)

best regards,

jannnesss
jannnesss is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45
CFX Post: Problems with moving point cloud for changing time steps spatialtime CFX 0 December 7, 2009 05:56
Inlet Velocity in CFX aeroman CFX 12 August 6, 2009 18:42
in CFX, how to define a inlet condition of feedback control flow rate ? suihenry CFX 12 May 14, 2009 17:59
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 06:13


All times are GMT -4. The time now is 18:15.