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

Can anybody please check my boundary conditions?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 3, 2011, 09:06
Default
  #41
New Member
 
Balakrshnan Ramakrishnan
Join Date: May 2009
Posts: 22
Rep Power: 8
Balakrshnan Ramakrishnan is on a distinguished road
do you use simpleFoam?

did you try to do without turbulence models?
Balakrshnan Ramakrishnan is offline   Reply With Quote

Old   August 3, 2011, 09:08
Default
  #42
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 463
Rep Power: 9
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
I only tried simpleFoam with turbulence models.
lovecraft22 is offline   Reply With Quote

Old   August 3, 2011, 09:10
Default
  #43
New Member
 
Balakrshnan Ramakrishnan
Join Date: May 2009
Posts: 22
Rep Power: 8
Balakrshnan Ramakrishnan is on a distinguished road
First : Try using no turbulence model. It will be easier to debug.

Second :

I cant understand why your k value is 0 everywhere and epsilon value is 1.78 ?? Any particular reason behind this?
Balakrshnan Ramakrishnan is offline   Reply With Quote

Old   August 3, 2011, 09:13
Default
  #44
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 463
Rep Power: 9
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
Quote:
Originally Posted by Balakrshnan Ramakrishnan View Post
First : Try using no turbulence model. It will be easier to debug.

Second :

I cant understand why your k value is 0 everywhere and epsilon value is 1.78 ?? Any particular reason behind this?
Nope, no reason, just copied them over from the motorbike tutorial. Anyway setting the boundary as srakshit I now got some reasonable results!

Thank you to both of you!
lovecraft22 is offline   Reply With Quote

Old   August 3, 2011, 09:17
Default
  #45
New Member
 
Balakrshnan Ramakrishnan
Join Date: May 2009
Posts: 22
Rep Power: 8
Balakrshnan Ramakrishnan is on a distinguished road
Just for your reference in the future simulations please look into

http://www.cfd-online.com/Wiki/Turbu...ary_conditions

to set initial conditions for k , epsilon and omega..

Have fun
Balakrshnan Ramakrishnan is offline   Reply With Quote

Old   August 3, 2011, 11:23
Default
  #46
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 463
Rep Power: 9
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
Thank you!
lovecraft22 is offline   Reply With Quote

Old   August 3, 2011, 22:53
Default
  #47
New Member
 
Sukanta Rakshit
Join Date: Jun 2009
Posts: 16
Rep Power: 8
srakshit is on a distinguished road
Quote:
You have to define one pressure value at least.

I set the pressure value to 0 at the inlet and the rest as you suggested.
Now it's running, let's see what comes out.
Out of pressure and velocity you can define one. If you have defined velocity at inlet and outlet as 30 m/s, then i wont prefer setting pressure = 0.

This is because of 2 reasons
1. If at the outlet U is fixed at 30 m/s, pressure will be depend on what fluid you are using. At steady state, both inlet and outlet pressure should be in the same range (not much difference) because its constant velocity simulation.
2. If U and p are inconsistent then you will get inconsistent solution. More iterations you will run, higher the velocity inside the domain you will get. This is because flow will bounce between two Dirichlet boundaries with inconsistent pressure.

If you are thinking of setting pressure in either of the boundary, then you have to keep the velocity floating at that boundary (or you should define some physical value).

Results with flow over a cylinder with fixed velocity (U=30 m/s) and floating pressure can be seen in the attached images.

Yes, i agree with Ramakrishnan. Turbulent properties should be defined correctly and solving without them will help in identifying the problem.
Attached Images
File Type: jpg freeStreamPressure.jpg (16.9 KB, 14 views)
File Type: jpg zeroGradient.jpg (15.3 KB, 14 views)
srakshit is offline   Reply With Quote

Old   August 4, 2011, 06:58
Default
  #48
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 463
Rep Power: 9
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
The same case won't converge with icoFoam… Why?
lovecraft22 is offline   Reply With Quote

Old   August 4, 2011, 19:40
Default
  #49
New Member
 
Sukanta Rakshit
Join Date: Jun 2009
Posts: 16
Rep Power: 8
srakshit is on a distinguished road
Quote:
Originally Posted by lovecraft22 View Post
The same case won't converge with icoFoam… Why?
It does, try decreasing the deltaT.

Also, check your ddtSchemes in fvSchemes.
srakshit is offline   Reply With Quote

Old   August 5, 2011, 04:24
Default
  #50
Senior Member
 
lore
Join Date: Mar 2010
Location: Italy
Posts: 463
Rep Power: 9
lovecraft22 is on a distinguished road
Send a message via Skype™ to lovecraft22
What should I check about the ddtSchemes?
lovecraft22 is offline   Reply With Quote

Old   August 5, 2011, 04:48
Red face
  #51
Senior Member
 
Mohammad
Join Date: Feb 2010
Location: Shiraz, Iran
Posts: 108
Rep Power: 7
m2montazari is on a distinguished road
hi,
as I had ran similar cases a lot, I think best condition is:
1- domain should be large enough and cell height at surface of cylinder should be small enough
2- boundary conditions should be as follows:
U: inlet: fixedValue, value=30,0,0
outlet: zeroGradient
cylinder: fixedValue,value=0,0,0
P: inlet: zeroGradient
outlet: fixedValue,value=0
cylinder: zeroGradient
k and omega: inlet: fixedValue,value=...(depend on your turbulence - you can use turbulence intensity instead of fixedValue also)
outlet: zeroGradient
cylinder:fixedValue,value=0 (for k)
fixedValue,value=a large number depending surface roughness(for omega)

3- discretization schemes should be limitedlinear or upwind (linear scheme makes fake pressure waves)

and about the pressure: most of CFD codes use gauge pressure to reduce errors because abs.pressure is usually a large number and its gradient is small, so roundoff errors increase with abs. pressure as calculation pressure. for incompressible cases as in N.S. and continuity eqn. there is no P, but just gradient of P, so any value for outlet pressure gives same result but a shift in pressure values in domain.

and about icoFoam, it is a piso based solver and should be ran with small timesteps. as your case has unsteadiness (because of vortex shedding and separation unsteadiness) you cant reach a steady converged solution but you can have converged unsteady solution after a reasonable time advance.

I hope these helps,
Mohammad
m2montazari 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
Impinging Jet Boundary Conditions Anindya Main CFD Forum 24 January 11, 2012 14:40
CFX does not continue Shafiul CFX 10 February 17, 2011 08:57
Proper Pressure Boundary Conditions for Buoyant Flow mchurchf OpenFOAM 0 March 25, 2010 13:16
Cell check and Boundary check errors AB CD-adapco 4 October 28, 2004 13:04
Please help with flow around car modelling! Tudor Miron CFX 17 March 19, 2004 20:23


All times are GMT -4. The time now is 10:37.