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

Tank emptying

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 28, 2012, 08:52
Default Tank emptying
  #1
Member
 
Andrea
Join Date: Feb 2012
Posts: 69
Rep Power: 5
Andrea1984 is on a distinguished road
Hi,

I'm trying to simulate the emptying of a tank with OF.
As I'm a newbie in OF, i have some doubt about the BCs.

The tank is 25x25 cm and has an height of 7 cm; the water height is equal to 5 cm and is drained through an hole at its bottom (d=1.3 cm).

The top of the tank is opened to atmosphere.

My doubt are about the boundary conditions for pressure and alpha1.

For the pressure I'm thinking to use a TotalPressure bc at the top (the same used in the DamBreak tutorial), zeroGradient at the outlet and zeroGradient at the wall (or should I use buoyantPressure for the walls?)

For alpha1 I want to use 0 for the top (only air), 1 for the outlet (only water) and zeroGradient at the walls.

Are this settings right?
Any tips about this particular case are welcome!

Thank you in advance.

Andrea
Andrea1984 is offline   Reply With Quote

Old   September 29, 2012, 05:35
Default
  #2
Member
 
Jan
Join Date: Dec 2009
Location: Berlin
Posts: 50
Rep Power: 8
SirWombat is on a distinguished road
Send a message via Skype™ to SirWombat
i suggest totalPressure for pressure at the outlet. make the water flow out to the atmospheric pressure (probably 0 if you haven't defined it) or use fixedValue = 0. you can use pressureInletOutletVelocity for the velocity at the outlet
SirWombat is offline   Reply With Quote

Old   September 30, 2012, 05:38
Default
  #3
nsf
Member
 
Nicolas Edh
Join Date: Mar 2010
Location: Uppsala, Sweden
Posts: 71
Rep Power: 6
nsf is on a distinguished road
Hi,

I would set inletOutlet on alpha1 on the outlet. If you on some point get a vortex which transports air out through the outlet you'll get into trouble if you prescribe a fixedValue.

Good luck!
nsf is offline   Reply With Quote

Old   October 1, 2012, 08:16
Default problem with total pressure = 0
  #4
New Member
 
Sam-CFD's Avatar
 
Sam Mathew
Join Date: Apr 2010
Location: India
Posts: 17
Rep Power: 6
Sam-CFD is on a distinguished road
On a sample problem, I've tried the same boundary condition on the bottom outlet as top atmosphere; which effectively means,

p_rgh (p - rho*g*h) being totalPressure

U being pressureInletOutletVelocity

alpha1 being inletOutlet

When I compare it to the analytical expression for the outlet flow rate and velocity {i.e., sqrt(2*g*h)}, the OpenFOAM results are around 1/3rd this value.

I performed the simulation in ANSYS FLUENT with Pressure Inlet (total gauge pressure = 0) and Pressure Outlet (static pressure outlet = 0) and the results seem to be acceptable to the analytical expression with some slight reduction due to viscous and other losses.

So, I am not quite sure if the boundary conditions suggested above are really correct?!

Any comments from others who have experience?

Thanks and regards,

Sam
Sam-CFD is offline   Reply With Quote

Old   October 1, 2012, 14:15
Default
  #5
nsf
Member
 
Nicolas Edh
Join Date: Mar 2010
Location: Uppsala, Sweden
Posts: 71
Rep Power: 6
nsf is on a distinguished road
Hi,

Have a look in
Code:
 ...tutorials/multiphase/interFoam/ras/waterChannel
In the tutorial, they set buoyantPressure for p_rgh on all patches except the atmospheric patch. Where the set totalPressure.

For U on the outlet it's inletOutlet.

They do set zeroGradient on alpha at the outlet. Which I think is fine unless there is any risk of reversed flow. In that case I would use inletOutlet.

Let us know how it goes!

/Nicolas
nsf is offline   Reply With Quote

Old   October 2, 2012, 05:18
Default
  #6
Member
 
Jan
Join Date: Dec 2009
Location: Berlin
Posts: 50
Rep Power: 8
SirWombat is on a distinguished road
Send a message via Skype™ to SirWombat
Quote:
Originally Posted by Sam-CFD View Post

When I compare it to the analytical expression for the outlet flow rate and velocity {i.e., sqrt(2*g*h)}, the OpenFOAM results are around 1/3rd this value.

Sam
When, how and where did you measure the velocity of the outflow? If no water is flowing into the tank then the velocity is a function of the height of the remaining waterlevel ... did you take this into account?
__________________
~~~_/)~~~
SirWombat is offline   Reply With Quote

Old   October 2, 2012, 09:09
Default
  #7
Member
 
Andrea
Join Date: Feb 2012
Posts: 69
Rep Power: 5
Andrea1984 is on a distinguished road
I have a fixed value for the flow rate at the outlet so I'm using a fixedValue for the velocity and zeroGradient for the pressure.

I think my problem is with the BCs at the wall, as I obtain a strange velocity field at the wall proximity using buoyantPressure (see attached picture, U contour at free surface).
Attached Images
File Type: jpg U_1sec.jpg (17.6 KB, 52 views)
Andrea1984 is offline   Reply With Quote

Old   October 3, 2012, 03:11
Default
  #8
New Member
 
Sam-CFD's Avatar
 
Sam Mathew
Join Date: Apr 2010
Location: India
Posts: 17
Rep Power: 6
Sam-CFD is on a distinguished road
Thanks for your responses.

I want to obtain the velocity at the outlet from the simulation and compare it with the analytical solution.
v = sqrt(2*g*h)
where, h = height of the liquid presently in the column.
Unlike Andrea's case, my problem involves a tank draining under gravity; therefore, I have to have a boundary condition on the outlet similar to static pressure = 0 (in ANSYS FLUENT).

I am expecting backflow at the outlet and gas to ingest into the domain. Primarily the aim is to verify whether, vortex from the top free-surface enters into the outlet.

Regards,
Sam

Quote:
Originally Posted by SirWombat View Post
When, how and where did you measure the velocity of the outflow? If no water is flowing into the tank then the velocity is a function of the height of the remaining waterlevel ... did you take this into account?

Last edited by Sam-CFD; October 3, 2012 at 05:52.
Sam-CFD is offline   Reply With Quote

Old   April 5, 2013, 10:29
Default
  #9
Member
 
Join Date: Mar 2013
Posts: 82
Rep Power: 3
giack is on a distinguished road
Hi to all,
I have a problem with the setting of the boundary condition in a similar problem.
My case is summarized as follow:
at the initial time t=0 the right wall of a closed tube completely filled with liquid is removed, allowing the liquid to exit the domain and, at the same time, allowing the gas to enter.
I set the BC in this way:
left wall: "p" zero gradient "U" fixed value (0,0,0) "alpha1" fixed value 1
pipe wall: "p" zero gradient "U" fixed value (0,0,0) "alpha1" zero gradient
right wall (outlet): "p" total pressure "U" pressureInletOutletVelocity "alpha1" inletOutlet
but I obtain unphysical result

Where is the error?Someone have an idea to set BC for this case?
thank to all
giack is offline   Reply With Quote

Old   April 5, 2013, 13:43
Default
  #10
nsf
Member
 
Nicolas Edh
Join Date: Mar 2010
Location: Uppsala, Sweden
Posts: 71
Rep Power: 6
nsf is on a distinguished road
Hi giack,

I once hade a problem with interFoam where alpha was unphysically diffused through the walls. This was resolved (for Of 2.1) by setting
Code:
    walls
    {
        type            buoyantPressure;
        gradient        uniform 0;
        value           uniform 0;
    }
on the wall patches. I think you should have zeroGradient on alpha on the left wall as well.

So for the patches that are walls (left and pipe) you should have the same bc's and they should be
velocity: fixedValue (0 0 0)
p_rgh: buoyantPressure (as above)
alpha: zeroGradient

I think the right wall is correct.

Good luck

Nicolas
nsf is offline   Reply With Quote

Old   April 7, 2013, 06:56
Default
  #11
Member
 
Join Date: Mar 2013
Posts: 82
Rep Power: 3
giack is on a distinguished road
thank you for your reply. I apply the suggestion that you give me but the problem remain the same...I think that there is something wrong in the set of pressure at the outlet but I don't understand what it is... Any ideas?
giack 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
Surge tank emptying using interFoam- Stops when surface reaches outlet Ramnik OpenFOAM Running, Solving & CFD 1 March 14, 2012 09:26
Surge tank emptying using InterFAOM- Stops when surface reaches outlet Ramnik OpenFOAM Running, Solving & CFD 0 May 26, 2010 11:42
Emptying tank & Multiphase Ruggero CD-adapco 18 October 24, 2007 13:23
How can i simulate a emptying bi-phasic tank? Ruggero FLUENT 1 July 9, 2007 03:17
Emptying of a tank Mario CFX 2 September 29, 2006 11:51


All times are GMT -4. The time now is 21:47.