
[Sponsors] 
December 8, 2010, 10:04 
two separation bubbles

#1 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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 

December 8, 2010, 18:13 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,857
Rep Power: 107 
Why do you think this is wrong? Are you sure this is not just a startup transient thing?


December 9, 2010, 00:21 

#3 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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 

December 9, 2010, 02:17 

#4 
Senior Member
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 11 
Hi Muhammad 
I modeled the T106A lowpressure turbine earlier this year and obtained pretty good results: http://www.cfdonline.com/Forums/cfx...sstmodel.html If you have any questions, please don't hesitate to ask. 

December 9, 2010, 03:47 

#5 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
hi Josh thanks for taking interest in my project,
can you give me your email address for further discussion? 

December 9, 2010, 08:19 

#6 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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? 

December 9, 2010, 08:24 

#7 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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? 

December 9, 2010, 08:50 

#8 
Senior Member
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 11 
Here's where I got the geometry from: http://wwwg.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 = 1.845E5 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. 

December 10, 2010, 05:33 

#9 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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 

December 10, 2010, 05:55 

#10 
Senior Member
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 11 
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 lowpressure turbine I think a minimum value of 1% is recommended.


December 10, 2010, 06:32 

#11 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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". 

December 10, 2010, 16:18 

#12 
Senior Member
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 11 
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.


December 11, 2010, 02:11 

#13 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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.... 

December 11, 2010, 06:24 

#14 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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.... 

December 12, 2010, 00:07 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,857
Rep Power: 107 
An image would help. Please post an image of the two separations and you general setup.


December 13, 2010, 02:32 

#16 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
I have uploaded it


December 13, 2010, 02:39 

#17 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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.... 

December 13, 2010, 02:42 

#18 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
This is the Velocity Vector Diagram....
Average value of Y+ on the blade is 0.0817 

December 13, 2010, 04:44 

#19 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,857
Rep Power: 107 
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? 

December 13, 2010, 07:14 

#20 
Member
Muhammad Aqib Chishty
Join Date: Nov 2010
Posts: 50
Rep Power: 8 
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 

Thread Tools  
Display Modes  


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 