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

[SuperSonic Nozzle] Bondary conditions of external domain

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 27, 2013, 04:37
Default [SuperSonic Nozzle] Bondary conditions of external domain
  #1
m_f
Member
 
M
Join Date: Jul 2012
Posts: 33
Rep Power: 4
m_f is on a distinguished road
Hello everyone,

I am actually realizing a study of a supersonic nozzle. With the method of characteristic, I design the shape of the nozzle to obtain exit Mach number around 2. When I run the problem without the external domain, the convergence is very quick and I obtain what i want.

Nevertheless, now I add the external domain, because I want to change the atmospheric pressure, to see if there are some shocks in different altitude.

So, I make this domain (see picture 1 in attachments), to simulate the atmospheric pressure.

Now, my question is : What kind of bondary conditions I have to use ? Pressure far-field ? Symetry ?
Everything I tried went to divergence.

Some informations about my problem.
All my BC are extracted from my MATLAB program using characteristic method.
BC 5 : Pressure Inlet
Ptotal = Pi = 70e+04 Pa
Ttotal = Ti = 500 K
Pstatic = 625534 Pa
Tstatic = 491 K

BC 6: Wall
BC 4: Axis

BC 1, 2, 3 : I don't know what is the optimum kind of bondary conditions ?
To be in optimum expansion condition, Pexit = Patm , my Pexit (static) is 77502 Pa.

Thanks by advance if you have any idea or suggestions.

Regards,
m_f

Note : Fluent 6.3 software
Attached Images
File Type: png picture1.png (45.3 KB, 61 views)

Last edited by m_f; May 27, 2013 at 10:25.
m_f is offline   Reply With Quote

Old   September 5, 2013, 16:14
Default
  #2
New Member
 
Obad
Join Date: Sep 2013
Posts: 29
Rep Power: 3
Obad is on a distinguished road
Hy!

I'm also currently working on programming over and underexpanded jet flow behind a laval nozzle. I have the same problem with the boundary conditions that you had. Did you manage to solve your problem? If yes, which boundary conditions did you choose?

Cheers!
Obad is offline   Reply With Quote

Old   September 7, 2013, 02:11
Default
  #3
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 7
duri is on a distinguished road
Did you tried pressure outlet for external BC 1,2,3
duri is offline   Reply With Quote

Old   September 9, 2013, 06:54
Default
  #4
New Member
 
Obad
Join Date: Sep 2013
Posts: 29
Rep Power: 3
Obad is on a distinguished road
Hy,
since I use Matalb to solve my problem I don't really know what pressure outlet means Does it mean that I have to define the static pressure at BC 1,2 and 3? Should this value then stay constant throughout the time steps?

But what about the other flow properties, should I simply choose arbitrary values for them to start and extrapolate the values at the boundary from the interior?

My approach was to use the characteristics to determine how many values should be variable at the boundary and how many should stay constant. For BC 1 which I assume to be subsonic this would mean that one characteristic plus the streamline goes inside my domain, hence I should keep 2 values constant and one variable. In my case the three variables would be the density, internal energy and velocity.

I'm really confused about this right now...
Obad is offline   Reply With Quote

Old   September 10, 2013, 04:41
Default
  #5
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 7
duri is on a distinguished road
Quote:
Originally Posted by Obad View Post
Hy,
since I use Matalb to solve my problem I don't really know what pressure outlet means Does it mean that I have to define the static pressure at BC 1,2 and 3? Should this value then stay constant throughout the time steps?
I replyed it for M. Where it seems he is solving this in fluent. Pressure oulet keeps the static pressure constant for subsonic outlet.

Quote:
Originally Posted by Obad View Post
My approach was to use the characteristics to determine how many values should be variable at the boundary and how many should stay constant. For BC 1 which I assume to be subsonic this would mean that one characteristic plus the streamline goes inside my domain, hence I should keep 2 values constant and one variable. In my case the three variables would be the density, internal energy and velocity.
density and internal energy is not the practical choice of boundary condition variable. Better use pressure and temperature, calculate density and internal energy from these variables.
duri is offline   Reply With Quote

Old   September 10, 2013, 06:05
Default
  #6
New Member
 
Obad
Join Date: Sep 2013
Posts: 29
Rep Power: 3
Obad is on a distinguished road
Thanks for your help duri!

Now I applied the pressure outlet as BC 1 and I treated BC 2 as a free slip wall. Since BC 3 is a supersonic outlet I extrapolate the internal values.
But it didn't work

Can you tell me if it is right to apply a free slip boundary condition to BC 2?
I'm also not sure if I apply this condition properly. For symmetry as well as free slip I put all normal gradients and the normal velocity component to zero.
Now, does a zero gradient e.g. at a symmetry mean, that the value at the symmetry simply becomes the value of the next internal node parallel to it?
Obad is offline   Reply With Quote

Old   September 10, 2013, 07:36
Default
  #7
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 7
duri is on a distinguished road
Quote:
Originally Posted by Obad View Post
Now I applied the pressure outlet as BC 1 and I treated BC 2 as a free slip wall. Since BC 3 is a supersonic outlet I extrapolate the internal values.
You can't simply apply extrapolation on one boundary and fix pressure on other boundary. Loop through cell and find local mach number to decide on extrapolation or pressure boundary.

BC1 is too close to nozzle exit, which could result in convergence issue. Its better to move it far upstream so that pressure at the boundary is not influenced by nozzle exit pressure.


Quote:
Originally Posted by Obad View Post

Can you tell me if it is right to apply a free slip boundary condition to BC 2?
I'm also not sure if I apply this condition properly. For symmetry as well as free slip I put all normal gradients and the normal velocity component to zero.
Pressure boundary is required for BC2. But, symmetry condition should not produce any difficulty in convergence. Symmetry will lead to nozzle efflux inside duct kind of physics. Symmetry and free slip conditions are same.
duri is offline   Reply With Quote

Old   September 10, 2013, 08:55
Default
  #8
New Member
 
Obad
Join Date: Sep 2013
Posts: 29
Rep Power: 3
Obad is on a distinguished road
Ok, I will try to expand boundary 1 in the upstream direction.

Did I understand you right that I should switch the boundary conditions at boundary 3 depending on the Mach number at each node at the exit? This would mean that when the Mach number at a node is supersonic I extrapolate ALL values from the inside and when the Mach number at a node is subsonic I apply
pressure outlet, hence the pressure becomes the specified static pressure and all other variables are extrapolated.
Since I'm performing a time marching calculation using maccormacks technique this means that the boundary condition at the same node can change with time.
is that right?
Obad is offline   Reply With Quote

Old   September 12, 2013, 14:38
Default
  #9
New Member
 
Obad
Join Date: Sep 2013
Posts: 29
Rep Power: 3
Obad is on a distinguished road
Update: I expanded my mesh in the outer region in the upstream direction and applied the following boundary conditions (see my attached figure for the labelling of my boundaries):

BC 1: Nozzle exit, all values are known and kept constant over time
BC 2: pressure outlet
BC 3: pressure outlet
BC 4: pressure outlet
BC 5: pressure outlet for nodes with subsonic speeds and simple extrapolation from the interior for supersonic nodes

BC 6: symmetry

BC 5 is the condition I'm most worried about.
Since my simulation diverges something must be wrong.

Can someone please tell me if this approach is appropriate, or what should I change?
Attached Images
File Type: jpg Skizze Randbedingungen.jpg (111.4 KB, 27 views)
Obad is offline   Reply With Quote

Old   September 13, 2013, 03:28
Default
  #10
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 7
duri is on a distinguished road
It seems you got confused a lot. Better try to solve this in softwares like fluent or cfx and understand what is happening before writing your own code.
This kind of BC2 and BC3 geometry is not much different from your old boundary. When you try to simulate a flow field try to match the geometry as close as possible.

It seems you are not simulating the nozzle flow. If is just nozzle exit as one boundary, then problem is quite simple keep the boundary adjacent to nozzle exit (top one) as wall. Keeping pressure inlet and outlet at adjacent cells won't work.
duri is offline   Reply With Quote

Old   September 13, 2013, 05:34
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,906
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by Obad View Post
Update: I expanded my mesh in the outer region in the upstream direction and applied the following boundary conditions (see my attached figure for the labelling of my boundaries):

BC 1: Nozzle exit, all values are known and kept constant over time
BC 2: pressure outlet
BC 3: pressure outlet
BC 4: pressure outlet
BC 5: pressure outlet for nodes with subsonic speeds and simple extrapolation from the interior for supersonic nodes

BC 6: symmetry

BC 5 is the condition I'm most worried about.
Since my simulation diverges something must be wrong.

Can someone please tell me if this approach is appropriate, or what should I change?
2 and 4 = wall with zero shear stress.

5 = pressure outlet with the required static pressure

3 = pressure inlet with total pressure=static pressure = static pressure at 5

6 = axis

7 = do not specify any boundary

other two boundaries should be pressure inlet and wall.
Far is offline   Reply With Quote

Old   October 14, 2013, 14:13
Default subsonic to supersonic nozzle flow coding
  #12
New Member
 
jatin kumar
Join Date: Oct 2013
Posts: 5
Rep Power: 3
jatin is on a distinguished road
hello everyone,
((subsonic to supersonic nozzle flow coding))

I want to write the nozzle length(x), area(a), density(r),velocity(v) and temperature(T) in non dimensional form (as the initial condition) in the MATLAB CODING..

please give me some hint to write these.......
thanks in advance............
jatin 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
How to sample a cut in domain which respects boundary conditions aerospain OpenFOAM 0 October 4, 2012 07:26
No results for solid domain Gary Holland CFX 10 March 13, 2009 04:30
Fan Boundary conditions with external analysis Rob FloEFD, FloWorks & FloTHERM 1 February 10, 2009 01:04
domain size for 3d external aerodynamics edi FLUENT 2 February 23, 2006 09:48
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 09:22.