Need help with CFX simulation for airfoil
 

Ok im now into using Ansys CFX solver after school they decided to change what we are using. I am running into a problem with defining my outlet boundary condition . The case is flow over an airfoil. I created the domain and extruded the geometry by 1. The geometry follows this tutorial by Cornell http://courses.cit.cornell.edu/fluent/airfoil/index.htm. When i run the case in CFX, I get this error for my outlet boundary. I have specified all the boundary type in Gambit but this "mysterious" wall is still in the geometry

****** Notice ******
| A wall has been placed at portion(s) of an OUTLET
| boundary condition (at 86.0% of the faces, 64.2% of the area)
| to prevent fluid from flowing into the domain.
| The boundary condition name is: Boundary 3.
| The fluid name is: Air Ideal Gas.
| If this situation persists, consider switching
| to an Opening type boundary condition instead.

Anyone has any idea on how to modify my geometry or know the exact problem? Thanks in advance.

1) this is the boundary condition problem in CFX.try to use opening as outlet boundary condition or extend the outlet to some extent.
2)In expert control parameters panel in CFX pre there is an option to avoid the artificial wall creation.set it to t

Hi,

It is a warning message. It is saying exactly what it says - there is backflow at your outlet so it has built artificial walls to stop this backflow.

If you are modelling flow over an airfoil this means your outlet boundary is too close to the airfoil. You need to move the outlet further downstream to a region where you are past the recirculations coming off the airfoil.

I don't recommend you use an opening or the expert parameter to hide this error. This will cause major inaccuracies in your simulation. The best approach is to move the boundary downstream.

Glenn Horrocks

Thanks for the suggestion. I tried changing the output pressure to a specific pressure and that solved the problem. Weird. I guess there are a few settings that i may have place wrongly. After changing it to be the same as the inlet that solved the problem. I assumed that there is 0 pressure changes within the domain. so i set the inlet and outlet pressure as the same Am i doing it correctly? Am new to CFD.

Hi,

You set the boundary conditions to match what you are trying to model! For most airfoil modelling you want to set the speed the airfoil is running at so a specified velocity inlet and a pressure outlet makes sense.

Glenn Horrocks

I am wondering if the inlet and outlet faces are defined as the same boundary since gradient is assumed as 0 for pressure and velocity across the inlet and outlet? I guessed it would not be possible since the mass flow need some boundaries to exit..

U are confusing me =). The gradient is 0 which i assume means that there the flow in the domain does not fluctuate much. And isn't setting the boundary determining where the flow goes in from and out from.

Would like to ask another question, the points on my airfoil are from standard coordinates found from the web. And when i plot the total pressure along with the x axis the curves are jagged is there a way to smooth it. Seems like exporting to excel does not help. Cant do much with the coordinates i have too. Lastly to find the coefficient of pressure on the airfoil which pressure value should i use total pressure or pressure. The help file is unclear about what is pressure alone.

Thanks.

Should be Pressure.

Hi,

To smooth the curves - Most solid modelling packages (including DesignModeller if that is what you are using) can fit a spline through points. This will allow you to smooth the curve and get a nicer pressure distribution.

Boundary conditions - As I previously said I think you will find a specified velocity boundary at the inlet and a pressure outlet will be what you are looking for. It is also a very stable configuration which will be easier to converge that pressure inlet and pressure outlet. Have a read of the documentation about boundary conditions.

Glenn Horrocks

Oh ok i get what you mean Thanks.

I would like to ask a question whihc may benefit some users. Its about timescales. I usually use the automatic timescale for simulation. But im curious about setting the Length scale option given. Im using the automatic timescale but when i use the conservative or aggressive length scale option. The post results are oscillatory and if i were to specify it myself with a scale of 0.00001 the oscillations are not there.

Can anyone recommend me where to read up on how to tune this. The help files are not really useful. Or can anyone suggest a setting to try out and guide me on how to tweak this. Thanks alot.

The effect are describe is explained here:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria

by the way, how to get the coefficient of lift and drag directly from the output? Is there an expression which I can key in?

I dont think so.

Hi,

CFX can output the force acting on a surface. You then use the definition of CD and CL (or CM or whatever you want) from there. Use a monitor point with the expression calculating CL or CD.

Glenn Horrocks

Was wondering if i should split the airfoil into 2 walls. And find the Forces in the y direction and x direction seperately, then add then together to find the lift and drag forces. So i can monitor both seperately. So splitting seems like a good option but im getting negative Y forces when adding the top and bottom surface.Think i will recheck my approach. Or is there any advice on a better way to do this. I am using the areaInt funtion to find the X and Y force, Direction none.

Did a test with the whole airfoil as one. And i would like to ask nother question which is if i use the funtion calculator and use the force function, with the Direction set to Global Y which force am i calculating.
Seems like there is a difference in both ways of calculating the force using areaintergration method and force function.

Also are the forces in the x and y inclusive of the wall shear stress?
Thanks alot.

Hi,

Use the force_x/y/z() function to get the force. This will then include contributions from both pressure (normal to surface) and wall shear (tangent to surface).

If you split the foil into a top and bottom surface then you can get the contributions from the top and bottom surfaces (obviously). If that is useful for you go for it.

Glenn Horrocks

Thanks alot for the help so far. Am learning much more now, smoothing out all the little details till i get a clearer picture of the software. The problem i have now is only the jagged pressure lines. I do not have modeler to smooth it out. But when i used the values below it is smooth.

The settings for the pressure are at fluid domain reference pressure = 1 atm, outlet static pressure,relative pressure = 0 Pa and inital condition relative pressure is at 0Pa. Followed the help files and tutorials on this settings. Turbulence model is Ke. Am doing a comparison on the various models too. Convergence was like only 40 iterations jagged all the way down. But force monitor was smooth. Output pressure readings was like only 5 Pa?? The velocity is low about 4.6 m/s. can it be considered as a converged result?

For all those interested in the Force calculation for lift and drag. This is what i did. Not sure if it is right but will post for reference,

Click the function calculator
Function Force
Location > Select Airfoil
Global > Y direction for Lift and X direction for Drag

Hi,

Smooth curves - some airfoil shapes have analytic shapes, such as the NACA 4 and 5 digit series. You don't need to fit splines to these, you can just use a finer resolution of the points defining the curve. Even if all you have is just coarse points then writing your own spline/curve fit equation is not too hard. Can do it in Excel if you have to. Then you can interpolate smoothly to fine points and get rid of the jagged pressure lines.

Boundaries - Are you using a velocity inlet?

Is it converged? - Good question. If you converge to a tighter convergence and the parameters of interest (in your case I guess that is CL and CD) don't change enough to worry you then, yes, it is converged.

Is it accurate? - Even better question. For the simulation to be accurate you need more than a converged solution. You need the correct physics, you need the boundaries far enough away to not affect results and you need a mesh fine enough to be accurate. A proper analysis will look at boundary proximity and mesh size and check the physics is correct.

Output forces - For airfoils it is very useful to define a monitor point with the CEL expression, something like force_x()@surface or whatever. Then you can monitor it as the solution converges and get a better feel for whether you have converged tight enough or not.

Glenn Horrocks

Yes im using a velocity inlet.

I understand what you mean by the convergence and curve refining. Thanks for the guide.
Now im going to to see if the pressure values are what it supposed to be and read about CEL expression kinda of confuse about it. Thanks.

Ok im getting a hang of it now.

Is there a guide on how to rotate the computational domain so that i can simulate the angle of attack. I tried changing the flow using Velocity*sin(angle in radians) etc. But the drag values turn out to be negative and it is not very good. Using a grid with y+ of 1 and results are not there. Therefore I want to learn to rotate the domain so that i can try out the results. anyone?

Thanks.