Low Reynolds Number SST Model
 

Hi all -

I am modeling the T106A low-pressure turbine, shown here:

http://img541.imageshack.us/img541/5...eometry.th.png

I am using the SST turbulence model. Here is my pressure distribution graph:

http://img401.imageshack.us/img401/1...fdvsexp.th.jpg

Ignore the orange line (Tu = 1%). Both the red and green lines (my initial results and my results with a quadrupled grid density, respectively) correlate alright with the experimental, but don't capture the laminar separation bubble on the suction surface (the experimental results have a pressure plateau).

At a recent fluids conference, a PhD student told me he obtained very good results (in comparison with Stieger's, found here: http://www-g.eng.cam.ac.uk/whittle/T106/Start.html) when he used the SST model with the low Reynolds feature turned on. I know the low Reynolds number feature exists in Fluent, but in CFX-Pre, I am unsure of how to turn off the automatic wall function.

After digging through the Help file, I have found many topics about the low Reynolds model, such as the required node refinement (at least 15 within the boundary layer for the low Re model, or 10 for the automatic wall function model), but I can't find any info on actually enabling the low Re model.

Does anyone know how to enable the low Re model and/or turn off the automatic wall function?

You results are very impressive, very good agreement with experiment, well done.

Rather than change the wall function approach why not turn on the turbulence transition model and try to directly model the laminar to turbulent transition? This will be your best bet to get even better accuracy in my opinion.

But if you REALLY want to change the wall modelling you will find the wall function options under the turbulence model in the domain tab. By default the SST mode has the automatic option enabled.

Thanks for the kind remark, Glenn. Unfortunately, my surface velocity and skin friction results aren't nearly as good.

I'll try what you said and post my new results. Thanks!

When I used the SST model without transitional turbulence, my solution did not converge, but it did oscillate very close to the residual values (and produced the above pressure results, which are pretty close to accurate). I didn't expect it to converge fully, as it is a highly three-dimensional, unsteady problem that I am modeling as two-dimensional and steady. When I tried using the transitional Gamma Theta Model, my residuals oscillated once again, but nowhere near the desired residual value.

A plot of y+ reveals maximum y+ values of 2.5 at the trailing and leading edges, and average y+ values < 1. Although CFX recommends a max y+ value of 1, the documentation said that results should not change significantly for 0.001 < y+ < 5, so a max of 2.5 seems reasonable.

CFX also recommended an expansion ratio of 1.1 with a hexahedral mesh, which I used.

I used the high resolution advection scheme, as recommended.

75-100 nodes in the streamwise direction are recommended. I used more, but that shouldn't drastically affect the results. They found that 30,000 nodes in most turbomachinery cases produces grid-independent results. I used just over 30,000 nodes.

I have read and practiced "obtaining convergence" on CFD Online, in the CFX Help file, and from various other sources. I will try a lower order discretization scheme, but I don't feel that will significantly help my solution converge. All I did was switch from the default SST to the SST with the Gamma Theta Model.

Any recommendations?

This comment is applicable to the default SST model. It is not applicable to SST with turbulence transition. The turbulence transition model requires a finer mesh, but you should do a sensitivity study to find out exactly how fine. You will probably have to lower the max y+ to about 1.

The turbulence transition model is often hard to converge in a steady state simulation. This is because you now have a transition, and for many airfoils you will get a laminar separation bubble associated with it (the transition model is very good at picking up laminar separation bubbles). However these bubbles are often unstable and jiggle about, even though the remainder of the flow is stable. This means you are forced to consider transient simulations.

Thanks again, honey (I heard that's what you're getting called these days).

I am trying to capture the laminar separation bubble, and I realize that this is an unsteady, three-dimensional problem in which the LSB likely fluctuates in size and location. However, I read a paper that was able to capture the LSB with steady, 2D simulations, so I thought I'd give it a whirl.

Yup, that's me :)

OK, but sounds like a problem to me. You might be really lucky with large timesteps that the turbulence model can stabilise it but you would need lots of luck. Your best bet is just to run transient.

Hey Glenn -

I tried the simulation with my original, unrefined (though higher quality) mesh, SST Gamma Theta Transition Model, and adaptive timesteps (with the initial, minimum, and maximum timesteps based on experimental data). I captured the LSB (teal line):

http://img72.imageshack.us/img72/176...phcfdvsexp.jpg

As for the location/size, we think my geometry is a little off (i.e. the incidence angle is incorrect) and that this is causing added acceleration over the suction surface. We came to this conclusion because:
1) The velocity profiles on the suction surface are too high and show an unexpected spike at about mid-chord. The acceleration should be somewhat constant.
2) My laminar separation bubble is small and delayed, which could be because of added momentum in the boundary layer due to the extra acceleration.

Thanks again, Glenn.

Just an update for your consideration. I changed the incidence angle from 37.7 degrees to 40.5 degrees and obtained much better results. I believe this is because the stagnation point on my geometry was improperly set.

http://img208.imageshack.us/i/cpsteadyunsteadytu1.jpg/

Boundary condition values
 

Hi Josh,
I'm doing the same analysis for the project. I checked and different sources i didn't find a good solution for the boundary value.

I have my value like given below.

Inlet
V=2.334 (for 1.6*10^5 re)
angle of Attack(37.7 deg)
x=2.33 cos(37.7)
y=2.33 sin(37.7)

but the problem is i didn't get the out let pressure value and the angle(do i need to consider angle on outlet pressure?)

i'm doing k and omega sst model

And the most worst case is i didn't get any bubble separation still now. my friends suggested the form. I hope i'll find some answer from you :)

Outlet reference pressure is zero if you're specifying an inlet velocity. I don't understand your "outlet angle" question.

You're not seeing bubble separation because you're not using the proper turbulence model. The k-w SST model failed to predict bubble separation (see the above graphs). The SST gamma-Re_theta transition model was what I used to predict the bubble, and an unsteady analysis was required.

thank you for setting me to the right track josh.. I'm doing my analysis in fluent and i'm new for CFD.

i calculated x and y by velocity triangle is this correct?
x=2.33 cos(37.7)
y=2.33 sin(37.7)
as the above post i'll change to 40.5 for my angle of attack.

I no longer have access to my simulations, but that looks correct. Post your results once you've obtained them.

really i was little relaxed :)

I'll update my result after i finish my computation.

Hi Josh,
i completed the solution and it is converged but i did't get bubble separation and i have reverse flow in face(some numbers) and on pressure out (some numbers)

i have attached you the jpeg files for reference. I can't figure why i have revers flow. I hope that you can help in this.

The reverse flow must be small. I cannot see it on your plots. Are you using Fluent? Any difference when you use CFX?

Hi,
I have not used CFX before. I think it should be same.

I showed to my professor and he told it fine but he asked me to make the bubble separation. i tried a little but i can't find it. I need some idea here i need to know where and what change. I'm new to CFD and fluent :(

This is the CFX forum so we cannot help you specifically with Fluent. I would try this model in CFX as I feel much more comfortable with that solver, but it is your choice. Also note Fluent has lots of different sovlers to try, if you use the coupled solver you will be closer to the CFX solver.

To get laminar separation bubbles you will need the turbulence transition model and a fine, good quality airfoil mesh.

Hi all,

I'm trying to do the same T106 analysis, but am not getting a correct velocity contour plot. I'm using inlet velocity of 8.45 m/s at an angle of 37.7. Just wondering if you guys have any tips for what I'm missing. Thanks very much.

FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

So you are simulating at Re = 1.15 * 10 ^ -05 based on inlet conditions that is roughly equivalent to Re = 2.3 * 10 ^ -05 at outlet.

I am using inlet velocity of 6.67 and angle 37.7 deg and taken these values from steiger's thesis and results are good enough with both transition models (k-kl-w and sst gamma-theta model)

Quick question relevant to this thread:

Where is the option to turn on low Re number modelling for the SST model? (See below). Is it in expert parameters? I certainly can't find it! :confused:

http://i.imgur.com/yE9qeqU.png

ensure Y+ < 6 and you have Low Reynolds no SST Model

Off course! :o

Be careful here - what Far is talking about is the wall boundary conditions. At the y+=6 approx is the transition from wall function approach to integration to the wall. But this only affects the wall boundaries. In the bulk flow there are turbulence models specifically designed to handle low Re flow where the turbulence intensity is low. That is a totally different thing and requires you to use a different turbulence model. There are low Re k-e turbulence models but CFX does not have them built-in, the low-Re turbulence models CFX has are the k-w series of models, including SST.

Thanks Glenn, I just clicked on this thread to query this. Alarm bells started to ring when Far mentioned Y+ must be < 6, which is fine for near wall flows however may not be valid for flows far away from the wall.

Let's say I'm simulating low Re turbulent flow, and I select the SST model.

In the turbulence options in CFX Pre is there an option I would need to click to tell CFX that I am simulating low Re turbulent bulk flow?

No, the default SST model can handle low Re well. The only thing is if there is transition you might consider adding the turbulence transition model.

But the turbulent transition model has been designed for external flow, no? So it may give misleading results if you switched it on for say something like flow in a pipe?

As we know SST model is combination of KW and KE model. So it has the capability to handle all type of flows well. If you have yplus between 1 and 20 (Y+ always vary on wall surface in real problems), automatic wall treatment will take care of it.

As far as SST transition model is concerned, it should work well for internal flow well. One good example is low pressure turbine transition prediction through SST transition model.

Mr CFD's concern is valid - the transition model was developed based on turbulence transition on airfoil sections/turbomachinery blades. So using it for other flows needs to be done with care and a validation before using it is wise. So I would not say it is misleading for other flows, I would just check it for your flow before using it.

Hi

I am attempting to match the experimental plot by steiger for Cp with my CFD simulation for T106. My results are

http://i57.tinypic.com/jpydyo.jpg

I am using Transition SST with turbulence intensity 0.4. Inlet Re No. is around 91000 and flow is operating at 1 atm. The problem is as you can see the peak of my Cp (around Axial Chord 0.6) does not match peak of Steiger's Cp plot (around Axial Chord 0.45). I have seen quiet a few CFD results of the problem and realize that CFD calculates the peak of Cp curve accurately. What do you suggest might be wrong with my approach that I am not being able to obtain better results?

First of all, I have no idea what T106 is. Please don't assume everybody understands your jargon.

And your question is an FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

@ Ghorrocks.. I am sorry, I thought as this thread started with discussion of modelling a T106 low-pressure turbine, it would be obvious, but I see its a year old thread so I should have given more detail.

No problem :)

Your results are not very far from the experimental results so I would hope mesh sensitivity checks, followed by checking your inlet conditions (especially the turbulence parameters at the inlet) would allow you to get very close. Of course the FAQ I linked to also said this (but in a more general fashion).

Hello,
Try to refine your mesh it should work. What is your Y+? for your case it should be below 2 if i remember correctly. try to refile the mesh of Y+=1

I have a hybrid mesh with a max y+ of 0.8.

Got the issue with the Cp curve resolved. However I am having some results I am finding hard to understand. I was taking 6.72 m/s as inlet velocity and 0 Pa as outlet pressure with 101325 Pa as operating pressure. However, when I change the operating pressure to zero and outlet pressure to 101325 Pa, my results got closer to the experimental results. Can anyone help me understand why that happened or if having operating pressure equal to zero and outlet pressure equal to 101325Pa is consistent with the physics of the problem?

Following are my Cp curves

http://i58.tinypic.com/24echua.jpg

I suspect this is just luck. Reference pressure = 101.3kPa, outlet = 0 is the recommended way to proceed as it reduced round off errors. If changing this to Ref pressure 0kPa, outlet = 101.3kPa changes things then your model is sensitive to small numeric changes and that is not good.

So I think you have a problem with inadequately resolved numerics and should fix that problem before trying to compare results. Are you using double precision? Also try running with a higher quality mesh.

I was using single precision, Maybe double precision will resolve the problem.. Checking it now