Different results in CFX with the same configuration on same airfoils made in solidwo
 

I ran two 3D simulations in CFX on NACA 23012 with 20 degrees angle of attack. One model was made in solidworks and then the airfoil was rotated 20 degrees and after that imported into the CFX simulation. In the CFX-pre expressions I didn't enter any angle of attack cuz it was already rotated.

The other model was made in DesignModular with the same dimensions and domain. The only different was that the airfoil was not rotated so in the CFX-Pre I applied the angle of attack in expressions to get lift and drag.

Apart from the airfoil rotation and the expressions applied all the configurations such as domain, inlet pressure, outlet, speed, density and everything were the same, but I got completely different results out of the simulation.

I was expecting to get the same results cuz in practice they are the same.
Well the both simulation results did get even close to the wind tunnel testing result I made on the same airfoil with the same dimensions.

Any idea as why these two give different results?

Check the mesh
 

1)Different CAD system make different parting line between surface. Next to the parting line the mesh could grow denser (if you don't take proper action to avoid this phenomena in the mesher program). The mesh generated is exacly the same?
2)What kind of mesher are you using?
3)What kind of fluid model you choose?
4)Is the fluid domain big enough around the airfoil?
5)Did you made a y+ estimation based on the Re number?
6)Did you consider inflation layer?
7)What about residual and imbalance?

This question is really an FAQ. What you are doing is comparing one inaccurate simulation to another inaccurate simulation and finding they don't match - no surprises there. SO what you need to do is the standard checks to make sure the simulations are accurate before you compare it to anything.

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

Thanks guys for the reply.

MB72
My domains are large enough for the laminar flow... the models were made in solidworks but the domain and meshin were made in ansys and they were exactly the same.
I have calculated the boundary layer and estimated the Y+ correctly.
The residual was converged on 1e-6 and the imbalances were less than 1%

ghorrocks
I've had a wind tunnel test by myslef in the lab on the same airfoil with the same chord and span so I have the real data to compare with... I'm not comparing the two inaccurate simulations with each other.
Apart getting two different values for the same model... I also get inaccurate results compare to the wind tunnel results, so there're two issues.
I've tried different settings but I never got close to the wind tunnel data.

These are the same airfoils in ansys designmodular... one rotated 20 degrees

Have you checked your mesh resolution is OK? Inadequate mesh resolution is one of the commonest mistakes.

Have you checked your airfoil geometry is not facetted? Designmodeller is famous for facetting the subtle curves in airfoils.

Can you post an image of your flow domain, the mesh around your airfoils and your CCL.

Well the mesh is not the best mesh but it's over 0.1 in orthogonal method which is in an acceptable range... if I wanted to make it more accurate then for a small change of quality there mesh elements would go from a million to beyond 5 millions. I made C shape and rectangular shape domain.
It's a laminar flow with 35m/s

Here are the pictures

Well

A)The only "escape way" is to rely on the huge amount of data gathered by NACA between the First and the Second WW.
Since you are managing a NACA profile, for sure you can rely on the their data. I think they developed some method to have a rough estimation of the Drag/Lift at various speed/angle of attack.
I think the book "theory of wing section" [Abbott] will help you a lot...
It will be interesting to compare the data of your lab with the NACA official results (which of course are assumed to be correct).

B)On CFX the only check you can perform is altering the mesh size and look if the solution change significantly.

C)If you have the chance, try to perform a quick 2D analisys with FLUENT: I'm not an expert but this solver can handle a "real 2D" simulation. CFX need 3D mesh, you have to trick it to perform something similar to a 2D simulation...

Let me know your findings

Now I have seen your mesh the reason is obvious. There is no way you are going to get good results with that mesh.
* It is far too coarse. You will need far more mesh resolution to get reliable answers
* The transition from inflation layer mesh to volume mesh involves far too large a change in mesh size. You need the mesh size to not have big jumps.
* You coarsen very quickly away from the airfoil.
* If this is a laminar flow then you do not need very fine resolution of the boundary layer as the boundary layer will be very thick.
* y+ calculations are meaningless for laminar flows. y+ is a turbulent flow thing only.
* You appear to have meshed the airfoil as a solid. Unless you are modelling heat transfer then you do not need to do this.

Your mesh quality and resolution explains why you are getting inaccurate answers.

oh sorry
maybe I'm wrong, but:
I've forgotten another Idea:
Are you studying the sistem as transient or steady? close to the stall the steady solution it is not fit. The big vortex behind the wing is basically unsteady, with evolution in time domain.
Close to the stall the aircraft starts "shacking"...

MB72
I've tried the 2D simulation in fluent with 2 millions of elements in mesh and I still get the different results... Unfortunately in the Wing section book the results don't cover the 3D simulation I try to run.
Those results are very old... the wind tunnel I had is a modern and computerised lab in our university so the data are accurate.
What I'm trying to do is that I've built the exact model in the wind tunnel for the ansys simulation and trying to trade off to find out where I get wrong.
There're other softwares for the 2D such as javafoil which gives a very good results and I don't even need ansys.

Ghorrocks
The model chord is 17cm and 0.36 m span.... the flow is laminar 35m/s, steady and the mesh is 1.2 millions of elements so for such a slow flow and such a small model this mesh should be enough... although it's not the best mesh but the result shouldn't be that far... wind tunnel lift is 98N and the simulation gives 21N...
There's a very weak turbulent occurs near the trailing edge which shouldn't have much effect on such a slow flow

just for curiosity:
what is javafoil predict about your wing? Is closer to wind tunnel result or not?
however is better to study the 2D profile in terms of Cd and Cl with ANSYS and correlate the results with NACA and javafoil data. After that you will correlate the results with wind tunnel data.
You need to write a plan before to try everything at the same time, therefore:
1)List all the computerized/non-computerized product you can use;
2)Use non-dimensional correlation at several point of the wing span;
3)Try to understand where the lack of lift pressure came from; is the pressure distribution around the wing consistent with literature data?

Let me know your findings

That sounds strange.
How do you enter an angle of attack as a CFX expression?
And how exactly does that alter the geometry or the mesh of an airfoil with initially zero angle of attack?

Javafoil is a free software here which uses Panel method to predict CL, CD, CM and etc... for different angle of attack.
The geometry is a simple airfoil so it's not complicated for mashing and I didn't check for the pressure cuz I need drag, lift and momentum which non of them give correct values, so if I get correct values on those then I might check for the pressure too :)

This's the whole CFX expression for NACA 23012 AIRFOIL on zero angle of attack model to get CL, CD and CM:

LIBRARY:
CEL:
&replace EXPRESSIONS:
AOA = 20[deg]
Denom = 0.5*massFlowAve(Density)@Inlet*Uinf^2*0.129295 [m^2]
Drag = cos(AOA)*Fx+sin(AOA)*Fy
Fx = force_x()@Airfoil
Fy = force_y()@Airfoil
Lift = cos(AOA)*Fy-sin(AOA)*Fx
Mz = torque_z()@Airfoil
Moment = Mx+My+Mz
Mx = torque_x()@Airfoil
My = torque_y()@Airfoil
Uinf = 35[m s^-1]
Ux = Uinf*cos(AOA)
Uy = Uinf*sin(AOA)
cD = Drag/Denom
cL = Lift/Denom
cM = Moment/Denom*0.18[m]
END
END

Maybe it's good for students to use it :)

---------------------------------------------------------------------------------------
Drag, Lift and Momentum are direct results of the pressure distribution on the wing.
Drag, Lift and Momentum are calculated by CFX calculator, starting from the integration of the pressure on the wing surface: the root is the pressure.
If you don't break this circle you will never be able to understand what's wrong.
Bye:)

As you said the Lift, Drag and Moment are the direct results of the integration of the pressure over the wing so when they don't give the correct results so it means the pressure value is not gona be correct too
:D
Thanks for the reply buddy

He he he. I cannot count the number of times I have been told that on the forum. Trust me, your mesh is the cause of the error.

Simply adding more mesh will not help. Have a look on the web at airfoil meshes (google it) and you will see some very nicely crafted meshes.