Hello everyone,

I'm working on a 2D simulation on a SD2030 airfoil using Spalart Allmaras model. The results will be validated on an established experiment; based on the lift and drag coefficient.

The results I obtained from my simulation using Fluent 6.2 were not convincing. The lift coefficients shows a promising result of 91% accuracy, and a similar trend but the drag coefficients were really far from the experimental value. For example; At Re 100 000, at alpha = 15deg; drag coefficient obtained was 0.145 where by the actual value was less than 0.05.

Another trend observed was that the viscous friction value was very small in relative to pressure coefficient right from the first simulation for 0 deg angle of attack. (I presumed that viscous friction should be more significant especially at 0 deg.)

I've tried grid adaptation, changing the grid, SIMPLEC solution, etc, but to no avail.

Could someone give me a reasonable explaination for such trend or errors; or an alternative solution to this?

Regards, Angela Bong

It's not surprising that you have more trouble with drag than with lift. That's usually the case. For high Reynolds number unstalled flow over a 2D airfoil, you can get pretty decent lift results even with potential flow. Considering that, I actually wouldn't be satisfied with almost 10% error in lift from a RANS method! That's a pretty large error which (along with your drag errors) signifies that something is seriously wrong...

As a first step to trouble-shoot this, I would compare the calculated pressure distribution with the experimental data (I assume they are available). If the pressure drag is off, as you say, you should be able to see that in the distribution. Maybe you get separation, where there was none in the experiments. Again, this would be visible in the pressure distribution. Only after knowing what's actually going on would I try to find a numerical remedy. Otherwise it's a shot in the dark.

Dear Mani, Thank you for your prompt advice. I just checked in the experiment report. Unfortunately, I do not have the calculated pressure distribution.

The experiment is not of my scope and I was referred to the experiment from my supervisor.

However, I realized that in the experiment, there were zigzag boundary layers added to the airfoil to simulate the effects of roughness caused by debris and erosion on turbine blades. For that reason, it is said that this would actually give a lower drag value property. Any hint on this?

And likewise, you were saying that you would not be even satisfied with 10% of error even with the RANS method. So, what would you suggest in light of this? Should I be simulating with a new turbulence model of higher transportation equation; such as the RANS method?

I would really appreciate your opinion.

Warmest Regards, Angela

Angela,

You said, "I do not have the calculated pressure distribution", but you probably meant you don't have the experimental pressure. What other experimental data are available?

The increased roughness on the surface would have the effect of triggering laminar to turbulent transition. If this reduces the drag, as the experiment report says, I can only imagine that there is a boundary layer separation somewhere on the airfoil. This separation may be reduced or delayed further downstream by increasing turbulence. Read the report carefully and try to find all information on the flow over the airfoil. If there is indeed separation, it will explain your difficulties. Does your RANS result show any separation?

Yes, of course, you could always try another turbulence model. If the result is quite different, you should examine the solution carefully and find the reason. This may give you a hint on what to focus in the experimental results.

Has the code been validated on any other airfoils? Your current case seems to be a little problematic.

Apologies if you have already done this, but I would strongly recommend that you:

(i) Perfrom a proper iterative convergence study.

(ii) Perform a proper grid convergence study (NOT grid adaption - the grid can only adapt to the structures that are resolved).

Although you don't have an experimental pressure distribution you do know at least one point (the stagnation point). Is your computed value sensible (is it one ? If not why not ?)

I'm with Mani - 10% error in lift seems way off the mark - even for Fluent.

Is there any reason you _have_ to validate your simulation against that particular experiment, other than the possibility that you're following your advisor's "recommendations"? Rather than spending so much time on convergence studies, various turbulence models, etc. etc., I'd strongly recommend that you look for "clean" experiments to validate your code against. I'm sure there are plenty of airfoil experiments to select from. If the issue is validation, try to minimize experimental ambiguities as much as possible. Right now you don't know where the problem is coming from - is there a bug in the code, is there a problem with the models you use, is there a convergene issue, is there an error in the experiment (_yes_ that is quite possible), does your simulation mimic experimental reality etc, etc.? You should strive to add complexities one at a time; otherwise, you'll be wasting months of valuable time and in the end you won't know, absolutely, what the underlying problem is ...

Adrin Gharakhani

Hi HelpfulSoul, Adrin, and Mani,

Thank you for the advices. Yes, I have to use this particular experiment as this experiment has aeroacoustic experiment results too. My objective is to investigate noise on this airfoil through CFD method. Therefore, unless I can validate its aerodynamic properties and its aeroacoustic properties, I can't use both results as a mean of correlation. I am supposed to correlate its noise to its pressure fluctuation.

My methodology is suppose to go this way: 2D aerodynamic simulation, 2D aeroacoustic simulation (which I am yet to explore), followed by 3D aeroacoustic simulation. It is actually a windturbine blade so the simulation is basically at low reynolds number. But given the time left, I am quite worried that I won't be in time to complete all these scopes. Now that one of you mentioned that 10% error is way out, I felt the need to further clarify my input in fluent. I started learning this in June, hence, my experience is still at infant stage.

Perhaps, I can consult any of you (Mani, HelpfulSoul, Adrin) personally via email? And we can further discuss in details. Maybe one of you can help me evaluate my fluent files.

Thank you in advance.

Warmest Regards, Angela

I don't use fluent so I don't know what it can and cannot do (correctly). I can tell you, however, that generally speaking, you're going to have a hard time getting any meaningful results for aeroacoustics using basic cfd codes. The first and second order algorithms (for cfd) offerred by fluent will most likely be insufficient. If you're having difficulty with a "simple" flow simulation of airfoils wait till you start with the acoustics component!

Adrin Gharakhani