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

two separation bubbles

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 8, 2010, 10:04
Post two separation bubbles
  #1
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
hi
i am simulating the Cascade T106 using the SST model. I am running an unsteady case. For few hundreds iterations i found more than one separation bubble. There is something wrong i thought. Can anyone give me opinion?

Regards:
Aqib
aqib is offline   Reply With Quote

Old   December 8, 2010, 18:13
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Why do you think this is wrong? Are you sure this is not just a startup transient thing?
ghorrocks is offline   Reply With Quote

Old   December 9, 2010, 00:21
Post
  #3
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
hi ghorrocks,
actually in most of the papers one separation bubble is mentioned, but in my case it show some different behavior. More than one separation bubble?
that is quite interesting for me.
thanks for reply
aqib is offline   Reply With Quote

Old   December 9, 2010, 02:17
Default
  #4
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
Hi Muhammad -

I modeled the T106A low-pressure turbine earlier this year and obtained pretty good results: Low Reynolds Number SST Model

If you have any questions, please don't hesitate to ask.
Josh is offline   Reply With Quote

Old   December 9, 2010, 03:47
Default
  #5
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
hi Josh thanks for taking interest in my project,
can you give me your email address for further discussion?
aqib is offline   Reply With Quote

Old   December 9, 2010, 08:19
Default
  #6
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
hi ghorrocks,
At the starting i have found 3 bubbles but after few thousand iterations only one bubble is left. Could you explain this phenomenon that why this happens?
aqib is offline   Reply With Quote

Old   December 9, 2010, 08:24
Default
  #7
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
hi JOSH,
i want to ask few things. First where you get the geometry of Cascade T106A? Secondly, i have some problem regarding inlet boundary conditions. I am taking the velocity inlet and pressure outlet, i am in the right direction? What value of Turbulence intensity is to be used?
I read soo much papers on Cascades but i cant specify the inlet conditions. Could you help me regarding that?
aqib is offline   Reply With Quote

Old   December 9, 2010, 08:50
Default
  #8
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
Here's where I got the geometry from: http://www-g.eng.cam.ac.uk/whittle/T106/Start.html

You can also find Stieger's published work at that site. That's where I got my boundary conditions from. I used a velocity at the inlet and a pressure at the outlet.

I calculated the exit velocity, based on work that was carried out at Whittle lab, and I came up with the exit velocity of 14.84 m/s. I used air at 26.5C (density = 1.17 kg/m^3, dynamic viscosity = 1.845E-5 kg/m.s). Since the axial velocity had to stay the same between inlet and outlet flows, I drew the velocity triangles. Based on the outlet flow angle of 63.2 degrees, inlet flow angle of 37.7 degrees, and outlet velocity of 14.84 m/s, I calculated the inlet velocity of 8.45 m/s. This gives a velocity ratio of 1.76, which is different than the published value of 2.01, but the published data were obtained under compressible conditions.

My pressure at the outlet was 0 relative to the 1 atm inlet pressure. This was not based on experimental work.
Josh is offline   Reply With Quote

Old   December 10, 2010, 05:33
Post
  #9
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
While setting the turbulence parameters at inlet and oulet boundary conditions there are many options available for example: Intensity and length scale, Intensity and viscosity Ratio. I know the turbulence intensity at inlet but i don't know how to select the length scale. If i am using ("Turbulence viscosity ratio") what value is recommended at inlet and outlet boundary conditions.
Regards:
Muhammad Aqib Chishty
aqib is offline   Reply With Quote

Old   December 10, 2010, 05:55
Default
  #10
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
If I'm not mistaken, the Stieger report actually gave a turbulence intensity and a turbulent length scale. Otherwise, a turbulence intensity study may be required. It's a difficult parameter to set, but for a low-pressure turbine I think a minimum value of 1% is recommended.
Josh is offline   Reply With Quote

Old   December 10, 2010, 06:32
Default
  #11
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
Thanks for replying again John,

I read the Stieger report and found
Ta=Tu(theta/L)^(1/5)
where,
Ta=Taylor's turbulence parameter
Tu=Turbulence Intensity
theta=Momentum thickness
L= turbulent length scale

i know the value of Tu=1%
but others thing are creating problem for me to specify the "L".
aqib is offline   Reply With Quote

Old   December 10, 2010, 16:18
Default
  #12
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
If it's not in Stieger, I'm not sure where I read it, but I specified "L" as 0.02 m based on experimental data.
Josh is offline   Reply With Quote

Old   December 11, 2010, 02:11
Post
  #13
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
I run my unsteady case.....
Time step size=0.001
Number of time steps:10000
Max iterations/Time step=100
When few thousands iteration runs, i found the separation but after 40000 iterations separation disappears. My Cd and Cl graphs shown me straight line. I don't know why separation disappear.... I am using Tu=5% and Turbulent length scale=1.
Please give your opinion....
aqib is offline   Reply With Quote

Old   December 11, 2010, 06:24
Unhappy
  #14
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
I am attaching my Cp result having a chord length of 0.198m
I cant understand what results are coming... Still, More than one separation bubble... How it could be....
aqib is offline   Reply With Quote

Old   December 12, 2010, 00:07
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
An image would help. Please post an image of the two separations and you general setup.
ghorrocks is offline   Reply With Quote

Old   December 13, 2010, 02:32
Post
  #16
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
I have uploaded it
Attached Images
File Type: jpg cp2.JPG (15.2 KB, 23 views)
aqib is offline   Reply With Quote

Old   December 13, 2010, 02:39
Default
  #17
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
Hi Ghorrocks,
I am using Velocity inlet and pressure outlet. Inlet velocity of 8.45m/s with inlet angle 37.7 degree. Taking Turbulence Intensity 0.1 and Turbulent Length Scale 0.02. Intermittency=1, using Pressure Velocity Coupling (Scheme) PISO.
Running and Unsteady Case with time step of 0.1 and Max iterations/Time step=100.
Also attaching my Velocity Vector Diagram....
aqib is offline   Reply With Quote

Old   December 13, 2010, 02:42
Post
  #18
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
This is the Velocity Vector Diagram....
Average value of Y+ on the blade is 0.0817
Attached Images
File Type: jpg Contours.JPG (63.5 KB, 23 views)
aqib is offline   Reply With Quote

Old   December 13, 2010, 04:44
Default
  #19
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
These are just laminar separation bubbles. They are often highly mobile transient things even when the rest of the flow is steady state so I doubt your steady state run has converged to this, but it is a transient state which will pass.

Also, what do you mean you are using PISO? This is not an option available in CFX.

I can't remember if intermittency=1 means turbulent or laminar, I suspect turbulent (I have not done a transition model for some time). Are you sure you want you inlet turbulent?
ghorrocks is offline   Reply With Quote

Old   December 13, 2010, 07:14
Default
  #20
Member
 
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 6
aqib is on a distinguished road
Hi ghorrocks,
In my steady state my Cd and Cl graphs are fluctuating.... that's why i am doing Unsteady Case....
Intermittency=1 means flow is turbulent and for '0' it means flow is laminar.....
"No actually in start my flow is laminar after that, separation happened and then flow reattached and becomes turbulent."
so initially my flows laminar....
that is the thing which i want to simulate
aqib 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
wall function and flow separation O.D.Y. FLUENT 1 October 3, 2011 16:27
Viscous model problem with bubbles in multiphase Shin FLUENT 0 March 10, 2008 18:31
Bubbles in vertical pipeline JM Main CFD Forum 1 March 9, 2007 14:11
Bubbles Søren CFX 0 April 12, 2002 04:01
Euler + separation again Oliver Main CFD Forum 23 June 19, 2001 12:47


All times are GMT -4. The time now is 13:43.