CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   two separation bubbles (

aqib December 8, 2010 10:04

two separation bubbles
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?


ghorrocks December 8, 2010 18:13

Why do you think this is wrong? Are you sure this is not just a startup transient thing?

aqib December 9, 2010 00:21

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

Josh December 9, 2010 02:17

Hi Muhammad -

I modeled the T106A low-pressure turbine earlier this year and obtained pretty good results:

If you have any questions, please don't hesitate to ask.

aqib December 9, 2010 03:47

hi Josh thanks for taking interest in my project,
can you give me your email address for further discussion?

aqib December 9, 2010 08:19

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 December 9, 2010 08:24

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?

Josh December 9, 2010 08:50

Here's where I got the geometry from:

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.

aqib December 10, 2010 05:33

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.
Muhammad Aqib Chishty

Josh December 10, 2010 05:55

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.

aqib December 10, 2010 06:32

Thanks for replying again John,

I read the Stieger report and found
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".

Josh December 10, 2010 16:18

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.

aqib December 11, 2010 02:11

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 December 11, 2010 06:24

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....:(

ghorrocks December 12, 2010 00:07

An image would help. Please post an image of the two separations and you general setup.

aqib December 13, 2010 02:32

1 Attachment(s)
I have uploaded it

aqib December 13, 2010 02:39

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 December 13, 2010 02:42

1 Attachment(s)
This is the Velocity Vector Diagram....
Average value of Y+ on the blade is 0.0817

ghorrocks December 13, 2010 04:44

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?

aqib December 13, 2010 07:14

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

All times are GMT -4. The time now is 20:31.