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

Flow in a tunnel

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   September 4, 2014, 10:45
Default Flow in a tunnel
  #1
New Member
 
Arthur
Join Date: Aug 2014
Location: Italy
Posts: 19
Rep Power: 2
Artur.Ant is on a distinguished road
Hello to everyone. I'm new with CFD and I need your help.
I try to simulate the flow around a train in a tunnel and for the beginning I created a long rectangular tunnel and imposed the boundary conditions: a velocity-inlet (40 m/s) and a pressure-outlet (0 pascal). (I used transient solver and k-w turbulent model). Can somebody explain me why the pressure near the velocity-inlet reach the maximum and decrease till reach the minimum near pressure outlet?
I also put a box (which represent the train) in the tunnel and the pressure is still maximum near velocity-inlet and decrease moving to pressure outlet. Also the minimum value reached by the pressure is in the back of my train. I expected a maximum value of the pressure in front of the train, but I got the maximum value for pressure near velocity inlet. Can anybody explain me why the pressure is maximum near the velocity-inlet and not in front of the train?
(To evaluate the pressure I used surface integral)
Artur.Ant is offline   Reply With Quote

Old   September 4, 2014, 15:30
Default
  #2
New Member
 
Adriana
Join Date: Sep 2014
Location: san jose, CA
Posts: 9
Rep Power: 2
adruma is on a distinguished road
Hello! I do not believe that you are supposed to impose what the pressure should be at the outlet. That will be calculated by the software. All you will have to do it to have your Cabinet open on all sides and apply the velocity BC on the inlet. The purpose of the CFD simulation is to calculate for you the N-S equations, which are pressure and velocity entities...

Regards,
Adriana D.
Aavid Thermalloy
San Jose, CA
adruma is offline   Reply With Quote

Old   September 5, 2014, 00:22
Default
  #3
New Member
 
Arthur
Join Date: Aug 2014
Location: Italy
Posts: 19
Rep Power: 2
Artur.Ant is on a distinguished road
Thank you for your replay. If I impose the velocity BC on the inlet what kind of BC should I impose on the other side of my Cabinet? I thought to impose an outflow condition, can it work in your opinion?
Artur.Ant is offline   Reply With Quote

Old   September 5, 2014, 01:01
Default
  #4
Member
 
le hoang anh
Join Date: Oct 2012
Posts: 96
Rep Power: 4
lehoanganh07 is on a distinguished road
I think you can try pressure-far field BC
lehoanganh07 is offline   Reply With Quote

Old   September 5, 2014, 01:12
Default
  #5
New Member
 
Adriana
Join Date: Sep 2014
Location: san jose, CA
Posts: 9
Rep Power: 2
adruma is on a distinguished road
What software do you use? If you use Icepak to simulate this, then you would have an opening on your cabinet at Inlet and Outlet (with velocity being applied at the opening at the inlet). All the other sides of your cabinet would be Default, or walls. If you use Fluent, then you apply velocity at the inlet, zero pressure on all sides except for the outlet. At the outlet you apply the "outlet" boundary conditions. I hope this helps.

Adriana

Aavid Thermalloy
San Jose, CA
adruma is offline   Reply With Quote

Old   September 5, 2014, 04:30
Default
  #6
Member
 
Anonymous
Join Date: Mar 2014
Posts: 57
Rep Power: 3
marauder is on a distinguished road
In theory it is correct as you are giving 0 pressure at outlet, inlet pressure should be more than 0 as there will be pressure loss in the system.

*sorry gave reverse info in last post :P

Last edited by marauder; September 5, 2014 at 06:24.
marauder is offline   Reply With Quote

Old   September 5, 2014, 06:14
Default
  #7
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Guys please...

For the setup you described so far (velocity inlet, pressure outlet) the results you obtained are physically valid. The reason is fluid dynamics.
Fluids flow from locations of high pressure to locations of low pressure. So if you impose a fluid flow from the inlet towards the outlet, pressure will be highest at the inlet.

I dont feel like I understand enough what you did after this first step to comment on the results. But I dont think that the setup you describe models the physical process correctly.
First of all, you should not impose a velocity. The flow velocity in the tunnel will be a result of the movement of the train. As a first approach, I would use pressure inlet and pressure outlet boundary conditions.
Then for the movement of the train it is not enough to impose a velocity on the walls of the train. You will have to model the movement with some kind of sliding mesh interface or a remeshing approach. Not an expert on this though so I cant give any further advice here.
ghost82 likes this.
flotus1 is offline   Reply With Quote

Old   September 5, 2014, 13:38
Default
  #8
New Member
 
Arthur
Join Date: Aug 2014
Location: Italy
Posts: 19
Rep Power: 2
Artur.Ant is on a distinguished road
Thank you for replys.
Flotus1 my interest is to calculate the difference of pressure between the front and the back of my train in tunnel. I can't use the sliding mesh technique because my computer can't handle a fine mesh.(I used a box of influence to create a fine mesh only near the train while for the far field I imposed the bigger size for mesh's elements) So to simulate the motion of the train in tunnel I considered a train at rest and a moving air. To move the air I imposed a velocity inlet and a pressure outlet but I'm not sure that these boundary condition can simulate, in the first approach, my case. Also the tunnel is quite long and the train is far from the inlet and the outlet. Can somebody tell me why these BC don't simulate correctly my case?
P.S. I use fluent.

Best regards.
Artur A.
Artur.Ant is offline   Reply With Quote

Old   September 5, 2014, 17:51
Default
  #9
New Member
 
Adriana
Join Date: Sep 2014
Location: san jose, CA
Posts: 9
Rep Power: 2
adruma is on a distinguished road
Try not to apply zero pressure boundary conditions at the outlet. I think your approach of moving air is good enough for what you want to simulate.

Adriana
Aavid Thermalloy
San Jose, CA
adruma is offline   Reply With Quote

Old   September 6, 2014, 09:35
Default
  #10
New Member
 
Arthur
Join Date: Aug 2014
Location: Italy
Posts: 19
Rep Power: 2
Artur.Ant is on a distinguished road
Is "pressure-far field" a better outlet condition in this case? And why?
Thanks

Best regards
Artur A.
Artur.Ant is offline   Reply With Quote

Old   September 6, 2014, 10:49
Default
  #11
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
I don't think pressure far field is a good bc for this problem; I would set a velocity inlet (air velocity=train velocity) and a pressure outlet (0 Pa gauge if the tunnel is open to atmosphere), or outflow BC.
If you don't use sliding mesh you are simulating a fixed train, like in a sort of a wind tunnel, where are moves instead of the train.
So, if this is your approach, and you want to study the train, I would increase the size of the domain and create a wind tunnel.
The bottom of the tunnel will be wall (no-slip velocity), side walls can be wall (no-slip velocity or zero shear stress)-->you can set also simmetry if side walls are far enough from the train.
Outlet should be far enough from the train, to let the vortices disappear and to not have reversed flow.
What Alex says is 100% correct, your pressure will be higher at inlet than outlet and you will have high pressure in the front of the train caused by the dynamic pressure.

Please post some pictures of pressure contour of the train.

PS: there are a lot of tutorials of cars in wind tunnels, you can read them and replicate your problem.

Quote:
Try not to apply zero pressure boundary conditions at the outlet. I think your approach of moving air is good enough for what you want to simulate.
I think this will be not usefull if boundaries are velocity inlet/pressure outlet: pressure values will be only shifted.

Daniele
ghost82 is offline   Reply With Quote

Old   September 7, 2014, 02:59
Default
  #12
New Member
 
Arthur
Join Date: Aug 2014
Location: Italy
Posts: 19
Rep Power: 2
Artur.Ant is on a distinguished road
To create my model I followed these steps:
1)created the train
2)created an enclosure (air)
3)created a boolean
so at this step I got just the air and the walls of te train inside it. After, when I created the mesh a used a box of influence to create a relative fine mesh near the train.
4)I created the walls for tunnel
5)I created the mesh for air and another one for the tunnel's walls

In this simulation I used sliding mesh tecnique but I tink that this is not very useful becaus me mesh is not fine enough. Is it correct? (You can see on the picture the dimensions of wall elements and air near the walls of the tunnel)
The setups are:
a)BC->velocity inlet = 40 m/s
b)BC->pressure outlet = gauge pressure = 0 pascal
c)BC->everything else are: stationary walls, interior (I got a symmetry plane in the midle of the tunnel to reduce the number of mesh elements)
d)cell zone condition ->walls of tunnel-> mesh motion 50m/s (so the walls of sliding mesh move at 50 m/s in the same direction of the velocity of the air)
e)the solver is : type=pressure based, time=transient
f)viscous model = standard k-omega
g)run calculation-> time step size= 1e-05
h)run calculation-> max iterations/time steps= 20
I used also a second order upwind for: momentum, turbulent kinetic energy, specific dissipation rate, tranient dormulation

On the pictures You can see the pressure contour on the train, symmetry plane, and planes just in front and back the train.
please give me your opinion.

best regards
Artur.Ant
Attached Images
File Type: png mesh.png (19.3 KB, 12 views)
File Type: jpg contour1.jpg (53.1 KB, 16 views)
File Type: jpg contour2.jpg (54.1 KB, 13 views)
File Type: jpg contour4.jpg (48.5 KB, 10 views)
File Type: jpg contour5.jpg (48.8 KB, 11 views)
Artur.Ant is offline   Reply With Quote

Old   September 7, 2014, 03:42
Default
  #13
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
You're setup is not correct.
Why for sliding mesh you are moving air and wall tunnel???
Only the Wall train and the mesh sourrounding the train must move, and you need to create interface between the mesh sourrounding the train and the external mesh.
However the problem is that you probably don't know for this configuration the boundary condition for air inlet.
I suggest to simulate the wind tunnel.
__________________
Google is your friend and the same for the search button!
ghost82 is offline   Reply With Quote

Old   September 7, 2014, 04:14
Default
  #14
New Member
 
Arthur
Join Date: Aug 2014
Location: Italy
Posts: 19
Rep Power: 2
Artur.Ant is on a distinguished road
The problem of train in tunnel is very similar to the problem of the elevator, and I found a document of a simulation of a high speed elevator. The author of that document said this about the sliding mesh: [quote: The “Sliding mesh” scheme has the elevator fixed in space while the walls and the fluid pass by at a constant speed]
So I decided to make the same thing.
Also the author of that document don't advise to make a dynamic mesh with the train in motion and the fluid and walls at rest because [quote: It is more numerically laborious and the scheme is only a first order accurate]

Can you confirm that a sliding mesh requires a very fine mesh?
Because in my document I want to report all the reason why I don't use a sliding mesh.
Thank you.

Best regards
Artur.Ant
Artur.Ant is offline   Reply With Quote

Old   September 7, 2014, 04:18
Default
  #15
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
Then, I don't get what is the advantage of using this type of sliding mesh instead of a static simulation with moving air.
Sliding mesh doesn't require particular fine mesh.
Are you sure the static elevator is using sliding mesh?Or it only moves air and wall tunnel without moving the mesh?In other words, is there only a fluid zone or are there 2 fluid zones connected by interface?
ghost82 is offline   Reply With Quote

Old   September 7, 2014, 04:19
Default
  #16
New Member
 
Arthur
Join Date: Aug 2014
Location: Italy
Posts: 19
Rep Power: 2
Artur.Ant is on a distinguished road
For the simulation of a wind tunnel in your opinion Should I keep the transient solver or not?
Artur.Ant is offline   Reply With Quote

Old   September 7, 2014, 04:23
Default
  #17
New Member
 
Arthur
Join Date: Aug 2014
Location: Italy
Posts: 19
Rep Power: 2
Artur.Ant is on a distinguished road
The author of that document report this advantage of a sliding mesh [ quote: This model has the correct relationship between the fluid and the hoistway walls]
The authors don't give any other explanation. They call it sliding mesh but don't give any explanation how they created the model or about the setups they used...
Artur.Ant is offline   Reply With Quote

Old   September 7, 2014, 04:42
Default
  #18
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
With sliding mesh transient solver is a must (obviously): for sliding mesh I mean 2 zones connected by interface, and one or both zones (meshes) are moving, sliding the interface.
For a wind tunnel static mesh I would try with steady solver; if the solution doesn't converge well (maybe because of vortices unsteadiness) I would switch to the transient solver from the steady solution.
ghost82 is offline   Reply With Quote

Old   September 7, 2014, 05:01
Default
  #19
New Member
 
Arthur
Join Date: Aug 2014
Location: Italy
Posts: 19
Rep Power: 2
Artur.Ant is on a distinguished road
Ok thank you.
I will try a simulation of a wind tunnel with a static mesh.
So to sum up:
I can use pressure outlet (pressure gauge 0) and velocity inlet (air velocity = train velocity) with the train and walls of the tunnel at rest.
Is it ok in your opinion?
Artur.Ant is offline   Reply With Quote

Old   September 7, 2014, 05:45
Default
  #20
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 918
Rep Power: 15
ghost82 will become famous soon enough
Yes, it sounds ok to me.
__________________
Google is your friend and the same for the search button!
ghost82 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
grid dependence, flow over a cylinder (inside a wind tunnel) dfmona CFX 9 March 21, 2010 20:47
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 104 February 16, 2006 06:44
Flow exit out of wind tunnel Peta FLUENT 1 February 3, 2006 10:15
Flow in wind tunnel Peta FLUENT 0 February 2, 2006 10:15
Kármán vortex street in cavitating flow behind bodies in the cavitation tunnel L. Könözsy Main CFD Forum 0 April 17, 2000 13:16


All times are GMT -4. The time now is 00:17.