Yet another NACA0012 Problem
 

Long time reader, first time poster.

I am required to investigate using CFD whether the height of our wind tunnel is enough so as not to effect the flow around a NACA0012 foil that resides within.

We have results from experiments to get the desired Cl and Cd values based on a series of Cp readings.

To begin with the geometry was created with a thin extruded duct and the aerofoil cut out. The issues started when it came to meshing it with CFX. Glenn Horrocks (Thanks for that information you sent) mentioned that it can be tricky to get inflation to continue to and round the trailing edge of the foil. The attached image shows it dying off as it approached the end.
The inflation layer itself goes from a prism height a fraction of the estimated boundary layer in height to the size of the other tetra cells. There is also constant face spacing along the foil surface.
Is there a way to get the inflation layers to continue round to the back?

The set up is a normal speed inlet, a zero relative pressure outlet. Global initilization has zero cartesian velocity components and a zero relative static pressure.

Also, in the results, I've created a polyline going along centre of the surface of the foil. Using this I'm plotting in a chart the pressure variance with distance. To get the Cp instead can I create a function or variable based on the pressure and use it as the chart variable?

Thank you very much for your time.

Regards,
Steven

Yes, you can do this.
Depending on wether or not you want to monitor this variable during the solver run, you have to specify this variable in CFX Pre before starting the solver run. In this case I believe you have to include this extra variable in the output list. This will make your solution file a bit larger, because the additional variable value will be stored for every grid point. Also you cannot monitor line plots during solver run, only scalar values.
Therefore it will probably suffice to define this variable in CFX post for evaluation.
You can simply create a new variable, define its value with a CEL expression and use it for evaluation on your line plot. It's pretty easym with the help of the manual you can probably figure it out in 5-10 minutes.

Good luck,

Jules

Hi,

A comment about your mesh. It looks like you have the airfoil as its own body. The inflation tool has problems at the trailing edge, that is why your inflation layers reduce to nothing at the trailing edge.

I recommend you put a thin cut out the end of the airfoil, and do an inflation mesh both sides of it. This will allow you to do a full thickness inflation layer right to the end of the foil. If you are clever you can also make the cut follow the airfoil wake then you will get much better modelling of the airfoil wake as you will be modelling it with prism elements not big tets.

Glenn Horrocks

The airfoil was an extruded cut from a 3D Curve generated from an external points file.
So you suggest cutting the duct during the geometry stage? Won't that effect the flow? Or do I just not assign a boundary condition to it in the solver?

Hi,

Yes, cut the duct in the geometry stage. You want a surface for the mesher to make prism layers on. But in CFX-Pre you merge the mesh back together again (this is recommended) or use an interface to re-connect them (not recommended).

Glenn Horrocks

I've taken a thin cut from the mid-section of the trailing edge of the foil and taken it all the way to the end wall, leaving the end face in two peices.

Do I need to create virtual topology during CFX mesh to merge the two surfaces back together again? I've looked through their help files and can't find a direct mention of merging two faces in CFX-Pre.

I tried an interface between the two and an alternative but it also spat out an error:

hey there.
lookin at your mesh, i was wondering if you tried to simulate a 2D-case? Because rightnow you didn`t have such. Your mesh isn´t periodic towards the sym-planes. Try the periodicpair option with one element thickness.

neewbie http://www.cfd-online.com/Forums/att...t-mesh-end.png

I found that periodic pair would throw up a lot of errors when I first tried it. It seems that was just a case of "ANSYS Behaving Badly".

Thanks for the tip neewbie, but after changing face spacing to edge spacing the number of mesh elements it stopped throwing up the error below but it doesn't impact on the cell resolution along the foil like it should. I change the edge spacing values but the cell size on the foil is only dpenedant on the minimum default face spacing size.

I'm also still unsure of the merging fo the faces in CFX Pre, I can't see any options for it.

Hi,

When meshing you should set it up as a 2D extrusion with 1 element thickness. In CFX you then define them as symmetry planes.

Also look here:
http://www.cfd-online.com/Wiki/Ansys..._simulation.3F

Glenn Horrocks

I have the front a rear walls as symmetry but you mentioned merging the top and bottom faces of the cut (Which was introduced to force the inflation layer to continue past the end of the foil) to form a single region.

At the moment the cut extending from the foil goes all the way to the outlet and slices it in half so I have two outlet regions.

Hi,

Two outlets should be fine.

Glenn Horrocks

But what about the two cut faces? I've tried setting them as interfaces, as symetry, as walls and in every case the solvre fails. Either due to an error
right away or after a couple of iterations because air is flowing back in the outlet.

You mentioned merging the faces or creating an interface, merging being the better option. How exactly does one merge the faces of the cut back together?

Hi,

The two faces can be merged in CFX-Pre. Providing the nodes match wither side then if you delete any wall it automatically generates and use a tolerancing thing hopefully you can do it. I have not done this for years so hopefully it still can be done!

If the nodes don't match or you can't figure how to do it then just use an interface.

Backflow are the outlet does not generally cause a solver failure. It might give a warning that artificial walls have been created. If this is the case then you probably have to move your outlet boundary downstream to be out of the wake zone. If your simulation is doing this does this mean the foil is stalled? You may need a 3D simulation with a DES approach to get any accuracy in the stalled region.

Glenn Horrocks

Thanks again for the help but it doesn't seem to want to work. In CFX-Pre, I assign walls, an inlet and outlet. I assign the two faces of the cut as walls and then try to delete them. They just return to "Default Domain Default" tree selection. I can click the box in front of it to hide them but the solver still takes them into account.

As for using an interface, I keep getting this error.

I have selected the top and bottom faces of the cut as the domain interface sides 1 and 2.