CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Simple Foam flow around airfoil

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   July 2, 2008, 03:54
Default Hi guys! It's my first post
  #1
New Member
 
Shemeck B
Join Date: Mar 2009
Posts: 5
Rep Power: 8
topik is on a distinguished road
Hi guys!

It's my first post on this forum, so welcome everybody 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 – symmetry ;
top and bottom – symmetry ;
airfoil – 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?

If you need more information about my analysis please ask.
Thanks a lot!!
Shemeck
topik is offline   Reply With Quote

Old   July 2, 2008, 04:07
Default Hi Shemech and welcome What
  #2
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,571
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
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
{
type zeroGradient;
}

Have fun,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   July 2, 2008, 04:12
Default hello! i 'm Hamdi N. I think
  #3
Member
 
hamdi
Join Date: Mar 2009
Posts: 72
Rep Power: 8
hamcer is on a distinguished road
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.
hamcer is offline   Reply With Quote

Old   July 2, 2008, 04:53
Default Yeah, for external, incompress
  #4
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
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.
madad2005 is offline   Reply With Quote

Old   July 4, 2008, 07:27
Default Hi! Thank you for your commen
  #5
New Member
 
Shemeck B
Join Date: Mar 2009
Posts: 5
Rep Power: 8
topik is on a distinguished road
Hi!
Thank you for your comments. I couldn't reply earlier beacuse I've been offline.
According to your advices I've setup new BC as follow:
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!
topik is offline   Reply With Quote

Old   July 4, 2008, 09:03
Default First of all, lift is generate
  #6
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
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.
madad2005 is offline   Reply With Quote

Old   July 4, 2008, 09:49
Default Adriano what do you mean by 'c
  #7
New Member
 
Shemeck B
Join Date: Mar 2009
Posts: 5
Rep Power: 8
topik is on a distinguished road
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 wrong
topik is offline   Reply With Quote

Old   July 4, 2008, 13:46
Default ah, ok. I didn't realise you h
  #8
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
ah, ok. I didn't realise you had already tried that.

"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).
madad2005 is offline   Reply With Quote

Old   July 4, 2008, 16:14
Default Hi Shemeck and all, In this
  #9
Member
 
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 8
paulo is on a distinguished road
Hi Shemeck and all,

In this link

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.
paulo is offline   Reply With Quote

Old   July 8, 2008, 03:26
Default Paulo thank you!! for your fil
  #10
New Member
 
Shemeck B
Join Date: Mar 2009
Posts: 5
Rep Power: 8
topik is on a distinguished road
Paulo thank you!! for your file it was helpfull.

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 is offline   Reply With Quote

Old   July 8, 2008, 03:53
Default Also I would like to plot cp d
  #11
New Member
 
Shemeck B
Join Date: Mar 2009
Posts: 5
Rep Power: 8
topik is on a distinguished road
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!!!
topik is offline   Reply With Quote

Old   July 8, 2008, 03:56
Default Hi Shemeck As you have p=0
  #12
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,571
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
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.

Hope it answered your question.

Best regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   July 8, 2008, 04:07
Default An example of a sampleDict is
  #13
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,571
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
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
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   December 8, 2008, 05:54
Default Go look at http://www.cfd-o
  #14
Senior Member
 
Wolfgang Heydlauff
Join Date: Mar 2009
Location: Germany
Posts: 136
Rep Power: 8
wolle1982 is on a distinguished road
Go look at

http://www.cfd-online.com/OpenFOAM_D...s/1/10206.html
wolle1982 is offline   Reply With Quote

Old   March 31, 2009, 09:04
Default HI Everybody
  #15
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 8
camoesas is on a distinguished road
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 is offline   Reply With Quote

Old   April 15, 2009, 09:59
Default
  #16
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 8
camoesas is on a distinguished road
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.
camoesas is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Simple foam solver mardinoglu OpenFOAM Running, Solving & CFD 1 October 17, 2014 04:56
Simple 2D airfoil Boudary Conditions doug OpenFOAM Running, Solving & CFD 3 November 9, 2009 11:32
Solve Simple foam for laminar flow nandiganavishal OpenFOAM Running, Solving & CFD 4 January 20, 2009 01:56
Flow Over Airfoil With Simple Flap Results fez FLUENT 3 February 23, 2005 11:56
Meshing An airfoil with a simple plain flap S. Kalam FLUENT 7 January 30, 2005 21:22


All times are GMT -4. The time now is 20:21.