two separation bubbles
 

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

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

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

Hi Muhammad -

I modeled the T106A low-pressure turbine earlier this year and obtained pretty good results: http://www.cfd-online.com/Forums/cfx...sst-model.html

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

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

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?

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?

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.

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

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.

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".

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.

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....

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....:(

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

I have uploaded it

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....

This is the Velocity Vector Diagram....
Average value of Y+ on the blade is 0.0817

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?

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

It looks like you posted an instantaneous Cp distribution. Those "multiple laminar separation bubbles" could be start-up/shedding vortices. If you average the Cp graph over time, you should obtain a better Cp distribution (the sharp spikes in the Cp graph should average to a plateau).

And a point from my previous post - what do you mean by PISO? This is not an option available in CFX.

PISO is actually present in Fluent 12.0.16 CFX.
The Pressure-Implicit with Splitting of Operators (PISO) pressure-velocity coupling
scheme, part of the SIMPLE family of algorithms, is based on the higher degree of the
approximate relation between the corrections for pressure and velocity. One of the limitations of the SIMPLE and SIMPLEC algorithms is that new velocities and corresponding fluxes do not satisfy the momentum balance after the pressure-correction equation is solved.

This is the CFX forum. Your question should be posted on the Fluent forum.

Any luck with the averaging?

How the averaging is being taken? I don't know about that!

now my graph of Cp is like that after taking the time step size of 0.001.

Yes, Aqib, I am well aware of what PISO and SIMPLE is. CFX only uses a coupled solver, very similar to the coupled solver in Fluent (the coupled solver in Fluent is from CFX technology, and for ancient history buffs the coupled solver in CFX came from Tascflow which was purchased by CFX years ago.)

i think you can't understand....

Can't understand what?

About PISO scheme

:) I am well aware of what the PISO scheme is. PISO is an option in Fluent, and is not available in CFX - and this is a CFX forum. So what don't I understand?

mine mistake :-)

That Cp graph looks much better. Did you average the Cp values over time?

are you talking about the single value averaged on the whole blade? Are you asking about the mean value of Cp plot over the complete flow time?
If you are talking about the first case then should i average the value on the vertex or facet?

I'm talking about Cp averaged over time.

i can't understand how to get that?
Did i take Facet Average over Blade?
How to take the Average Cp over time?

You'll have to export the Cp data at each timestep, which can be done with a batch file, then write a macro that averages all the Cp files.

I calculate the Pressure co-efficient value by two methods tell me which is right....
1. I record the Pressure co-efficient value and select the "Integral" in Report type option(In surface Monitor) and after 4.4239 sec my average value is: 0.467477514
2. I record the Pressure co-efficient value and select the "Facet Average" in Report type option(In surface Monitor) and after 4.4239 sec my average value is: 1.063549129
Tell me which method is right and which value is more accurate?

My Velocity Ratio is:
Vout/Vin = 1.779
is it ok?