CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   running airFoil2D (http://www.cfd-online.com/Forums/openfoam/67122-running-airfoil2d.html)

nomad August 4, 2009 19:34

running airFoil2D
 
Hi,
Why doesn't the airFoil2D case have a blockMeshDict? I tried running icoFoam on airFoil2D but the error message said that mesh description file could not be opened.
Do I need to create one, and if so, is there a way of generating vertices, blocks, patches,etc?
Thanks!

henrik August 5, 2009 02:22

Dear Nomad,

because the mesh is already ready for use.

Maybe the mesh has not been created with blockMesh, but has been imported from external sources.

Henrik

bigred August 5, 2009 02:58

I was wondering the same thing. Where is the Mesh information stored and can you just run the simulation then? ie. skip the blockMesh part and just type potentialFoam (or whichever one it was). Is the Mesh file editable in a mesh generator like netgen or gmsh?

henrik August 5, 2009 03:10

Dear Nomad,

please have a look into sections 5.1.1 and 5.1.2 of the user manual where is all explained in detail.

Henrik

bigred August 5, 2009 06:34

I just read through the user guide again (doh, should've done it first! Didn't recall that information from the first time I went through the guide) and it's a lot clearer.

nomad August 5, 2009 13:30

Thanks Henrik,
If I want to analyze my own airfoil, I would still need to write a blockMeshDict file to generate the boundaries, cells, faces, etc. data.
If so, how would I set up the vertices, blocks, and patches?
Or is it better to use an external pre-processor?
Thanks.

henrik August 5, 2009 13:56

Dear Nomad,

there is a bunch of converters which will read almost any mesh format. See here:

http://www.opencfd.co.uk/openfoam/me...meshConversion

I am also pretty sure that there are tools in the open domain to create meshes for the standard 2D airfoils ... browse the forum and web.

Henrik

nomad September 1, 2009 23:17

NGSolve airfoil mesh
 
1 Attachment(s)
Hi,
I've been getting pretty crappy results with an airfoil at a small angle of attack in openfoam, I'm using NGSolve to generate the mesh (which doesn't look very nice) and gmsh to optimize it and I've attached a picture of it. Is there anyway of improving the mesh in either NGSolve or gmsh and do I really have to use both?

Some help would be appreciated.

Thanks.

chbenz September 2, 2009 01:30

Hi,

why do you use tetraeder. I think a hexa-mesh would be much better.

Christof

nomad September 2, 2009 14:15

Hi Christof,
Would you be able to recommend opensource hex-mesh generators? It seems like CUBIT (Sandia) and CART3d (NASA) are restricted for use to only US citizens. Are there mesh generators that are catered towards airfoil meshes?
Thanks.

chbenz September 2, 2009 15:06

Hi,

you could try Salome or Netgen. If you google them you will find some tutorials. I think they are appropriate for airfoil mesh generation.

Christof

nomad September 2, 2009 15:09

I am using NetGen, the attached jpeg above is of a mesh created in NetGen, however I didn't know it could do hex meshes.

chbenz September 2, 2009 15:17

ahh....i see it only meshes tets automatically.
you can use Salome for hexa meshing.
Why you dont use blockMesh?

Christof

nomad September 2, 2009 15:33

In order to use blockmesh, if I'm right, you need to have the vertices of the volume already defined, including patches, blocks, edges, etc. If there is a trivial way of doing this for an airfoil, please do let me know.

chbenz September 3, 2009 00:03

youre right john. i dont know exactly but the surface of an airfoil is a analytical function, or? if so you could estimate the coordinates if all points. another way is to use snappyHexMesh.
nevertheless you could increase your volumenumber.

nomad September 4, 2009 13:47

So I suppose the reason I was getting crappy results with the airfoil at low angles of attack was because I was specifying the boundaries of the control volume incorrectly. The flow around the airfoil is an external flow and so maybe the walls should be assigned freestream values instead of fixed values.This still doesn't mean that the mesh is acceptable.
Anyway, I get the right flow, but I still don't get the right force values.
Also, since this is a 2d flow (single cell thickness of mesh), I should be able to plot streams in paraFoam. However, I only get 5 streams. How do I get more streams to show up?
Thanks

hansel September 7, 2009 16:58

Quote:

Originally Posted by nomad (Post 228598)
So I suppose the reason I was getting crappy results with the airfoil at low angles of attack was because I was specifying the boundaries of the control volume incorrectly. The flow around the airfoil is an external flow and so maybe the walls should be assigned freestream values instead of fixed values.This still doesn't mean that the mesh is acceptable.
Anyway, I get the right flow, but I still don't get the right force values.
Also, since this is a 2d flow (single cell thickness of mesh), I should be able to plot streams in paraFoam. However, I only get 5 streams. How do I get more streams to show up?
Thanks

I'm also working with foils in wind turbines and have been getting some strange numbers. One thing I've recently discovered is that the mesh size at the surface is very important. If it's too large the air slips right by with apparently no boundary layer and no friction.

I'm currently working with a simple cylinder to see if I can get reasonable numbers.

BTW I've been using gmsh to make my meshes. It's got a fairly nice language for describing the geometry, and I like that it slowly blends cell sizes from one point to another. I've seen abrupt changes in cell sizes cause problems with some of the solvers.

Steve

hansel September 7, 2009 17:02

Quote:

Originally Posted by nomad (Post 228598)
, I should be able to plot streams in paraFoam. However, I only get 5 streams. How do I get more streams to show up?
Thanks

I like to change the stream from point based to line based. Then there is a 'resolution' number which is the number of points along that line for starting streams. You can also move the ends of the line closer to the foil because you don't really care about the streams way off to the side.

Also the glyph display isn't bad for seeing the air flow. I usually change the default scale down by a factor of 10 because i have a big 10m x 10m test area and a foil that's only about 0.1 m long.

MadsR September 23, 2009 04:40

Hi Guys.

If you are working with a mesh like the one that's depicted a few posts up, a very crude tet-mesh, I am not surprised that you get more or less arbitrary results - at least when looking at surface-related integral quantities, such as pressure, lift and drag. And sadly, these quantities are typically of most interest.

You need to resolve the boundary layer, or have some really capable wall-models (at least for the attached case). A suggestion could be to mesh (with hexahedrals to reduce false interpolation, especially at the boundary), with y+ down to 1-3 at the airfoil. When meshing with such low y+ values, you need to remember to use a turbulence model which does NOT employ wall-models. Typically they are called low-Reynolds Number-models. A genuine implementation of the Spalart-Allmaras model should be OK at low angle of attack. Many other models are also applicable, as long as they do not use wall-models.

When the flow separates, at high angle of attack, you most definitely need this, and your milage may vary nonetheless as separated airfoil flows are among the most difficult problems to solve (and hence the most exciting). SAS-, DES- or even LES-approaches may be the only way there.

Just my 2 cents.
/Mads

hansel September 23, 2009 11:08

Thanks for all the pointers MadsR! I guess I need to step back and ask the big question... Has CFD and computer technology progressed to the point where you can put an untested virtual item in an airflow and know how it will behave in real life? I've been learning that to make simulation agree with known results takes much work, and there are 1000x more ways to get bad results than good ones.

My dream was to be able to put untested wind turbine designs in a virtual wind and see how they work. But this involves wings being at all angles of attack, some in stall, different wing speeds at different points of the rotation, etc. I'm starting to think CFD isn't there yet.

Maybe in 20 more years, when computers are 1000x faster, and we can do everything with a 10 micronmesh it might work.

Is CFD useful for testing cars or planes? Or is it only used to see what's happening when you get some strange wind tunnel results?

Any opinions would be appreciated.

Steve (Now thinking a wind tunnel is the way to go)


All times are GMT -4. The time now is 02:49.