CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Simple Foam flow around airfoil (http://www.cfd-online.com/Forums/openfoam-solving/58235-simple-foam-flow-around-airfoil.html)

 topik July 2, 2008 03:54

Hi guys! It's my first post

Hi guys!

It's my first post on this forum, so welcome everybodyhttp://www.cfd-online.com/OpenFOAM_D...part/happy.gif I'm new with OpenFoam and I met some problems during my calculations.

I'm running the case using the simpleFoam solver. it's a steady turbulent (k-epsilon) flow around the airfoil. Could you please have a look on my velocity distribution:

http://img234.imageshack.us/img234/2973/a0006ww5.jpg

boundary conditions are:
inlet - v=50, p=0 ;
outlet - p=0 ;
front and back &ndash; symmetry ;
top and bottom &ndash; symmetry ;
airfoil &ndash; wall,

I'm trying to find out what I did wrong but I'm struggle. Only in top left corner of the 'tunnel' something is happening, why?
Is it possible to obtain v = 2.00e+24 when the inlet velocity is 50?

Thanks a lot!!
Shemeck

 ngj July 2, 2008 04:07

Hi Shemech and welcome What

Hi Shemech and welcome

What happens is that you specify p=0 at both inlet and outlet. Thus to narrow it down you have a setup with a possible significant energy loss but a zero pressure gradient, thus it is a non-physical setup.

Instead you should set at the inlet a zeroGradient in p, i.e. type in /0/p

inlet
{
}

Have fun,

Niels

 hamcer July 2, 2008 04:12

hello! i 'm Hamdi N. I think

hello!
i 'm Hamdi N.
I think y'r in the exten flow not in intern flow, thus y can't use inlet or output boundary, y can see the tutorials of OF;

good luck.

Yeah, for external, incompress

Yeah, for external, incompressible flows you are better using a velocity inlet and a pressure outlet with symmetry everywhere else. There is also the option to use freestream boundary everywhere, since you are dealing with an isolated aerofoil. However, this may only be possible for compressible flow. Setting a mass-flow inlet is another option.

I'd recommend you increase the size of your farfield domain, though. They should be at least 10 aerofoil chord lengths away from the aerofoil itself. There have been many studies to show this too.

 topik July 4, 2008 07:27

Hi! Thank you for your commen

Hi!
inlet - pressureInlet v=100, p zero gradient
outlet - pressureOutlet p=0
I'm satisfied with pressure and velocity distributions, it follows my expectactions. But I'm not happy with values of pressure and velocities:
pmin = -1,6e13 (underpressure,how?) pmax = 4,92e+12
vmin=8,46e3 vmax=5,26e6
Those numbers are definitly to big, any ideas why?
I've also increased distance between inlet and airfoil.

thanks for help!

First of all, lift is generate

First of all, lift is generated on an aerofoil by integrating the pressure around it. You can get low pressure on the upper surface due to the aerofoil's camber and thickness (obviously a.o.a.). Your velocities don't look right though. Change p-inlet to v-inlet and see what you get.

 topik July 4, 2008 09:49

Adriano what do you mean by 'c

Adriano what do you mean by 'change p-inlet to v-inlet'? I've tried fixed v (Inlet boundary condition) at the beginning of my simulation, if this is what you mean.
I got 6 more initial inlet conditions to choose:
pressureInlet,
inletOutlet,
pressureInletOutlet,
freestream,
extrapolatedInletOutlet,
atmosphere.
I'have been trying one by one for a while and I always getting wrong values of velocity and pressure.
I know the principles of lift force generation but in my opinion it's not possible to obtain underpressure around the airfoil, but I might be wronghttp://www.cfd-online.com/OpenFOAM_D...part/happy.gif

ah, ok. I didn't realise you h

"inlet - pressureInlet v=100, p zero gradient "

This suggested you were still using a pressureinlet even, though you specified a velocity. I wasn't sure. By low pressure, I didn't mean negative pressure, no! :-)

Try freestream set to Vx = 50m/s front, back, top, and bottom, with symmetry only at the sides. Are you sure you have specified the surface name's properly? Maybe you've set the boundary conditions to the wrong surfaces? That would certainly cause you problems (i.e. inlet face set to symmetry and symmetry face set to velocity inlet).

 paulo July 4, 2008 16:14

Hi Shemeck and all, In this

Hi Shemeck and all,

http://www.posmec.ufc.br/~paulo/Open...perc_ke.tar.gz

we have a functional case of a flow around a cylinder, using k-e.

If it interests you, feel free to analyze it.

Regards,

Paulo.

 topik July 8, 2008 03:26

Paulo thank you!! for your fil

After few hours of investigation I found the boundary conditions which work in my case.

I've setup:
inlet - Inlet, p zero gradient, v=20m/s fixed value ;
outlet - Outlet, v zero gradient, p=0 fixed value.
airfoil - wallFunction v=0m/s
sides,top,bottom - symmetry
I've also assumed new values of k and epsilon and other solution scheme.

I was very surprised after few iterations because everything was fine. I'm very happy about velocity but values of pressure seem to be wrong.
For example:
after t=200 pmin = -940, pmax=1.31e3
t=3000 pmin = -544, pmax = 262

Now I'm a bit confused because I met some people in which opinion it's possible to obtain underpressure in case of flow around airfoil/cylinder. what's yours opinion?

 topik July 8, 2008 03:53

Also I would like to plot cp d

Also I would like to plot cp distribution on my foil. I went through user guide (chapter 7.5) but it's not clear for me how it works. Is there anyone who dealed with this particular case before? I would be very appreciate if someone could paste sampleDict file.
thanks!!!

 ngj July 8, 2008 03:56

Hi Shemeck As you have p=0

Hi Shemeck

As you have p=0 at the outlet, it is definitely not surprising, that you have positive and negative pressures.

Consider your problem in a loss-free environment, aka use the Bernoulli equation around your air-foil. Then you will get a large pressure at the upstream stagnation point and further you will get a drop in the pressure where the contraction of the streamlines is largest.

Further the pressure you specify is only relative, thus you could specify atmospheric pressure and you would not get negative pressures.

Best regards,

Niels

 ngj July 8, 2008 04:07

An example of a sampleDict is

An example of a sampleDict is to be found with the source at the following location:

~/OpenFOAM/OpenFOAM-1.4.1/applications/utilities/postProcessing/miscellaneous/sa mple

- Niels

 wolle1982 December 8, 2008 05:54

Go look at http://www.cfd-o

 camoesas March 31, 2009 09:04

HI Everybody

HI everybody!

I am new to OpenFOAM, to CFD and to this board, so please be patient. :)
I have a problem similiar to Shemeck, I am trying to simulate a flow around an airfoil. I have set the boundaries for U and p as follows:
p:
Quote:
 dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { inlet { type zeroGradient; } outlet { type fixedValue; value uniform 1; } frontAndBack { type empty; } pressureSide { type zeroGradient; } suctionSide { type zeroGradient; } leadingEdge { type zeroGradient; } trailingEdge { type zeroGradient; } passageSides { type symmetryPlane; } }
U:
Quote:
 dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { inlet { type fixedValue; value uniform (80 0 0); } outlet { type zeroGradient; } frontAndBack { type empty; } pressureSide { type fixedValue; value uniform (0 0 0); } suctionSide { type fixedValue; value uniform (0 0 0); } leadingEdge { type fixedValue; value uniform (0 0 0); } trailingEdge { type fixedValue; value uniform (0 0 0); } passageSides { type symmetryPlane; } }
These are the boundary conditions found to be appropiate above. Altough I do not get any flow. have a look:

http://img166.imageshack.us/img166/9734/26471311.jpg
http://img520.imageshack.us/img520/3057/17723107.jpg

So where is the mistake? Thank you for your help. Is there is any more information I have forgotten to post, feel free to ask.

Ps: As you can clearly see in the picteres my mesh is far from beeing perfect I am working on that. :(

 camoesas April 15, 2009 09:59

HI Everybody!

I have solved my problem by myself. It was the mesh indeed. I had mixed up only one point in blockMeshDict file.

My apologies for my ignorance.

 All times are GMT -4. The time now is 02:50.