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