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

interfoam BC

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

Like Tree2Likes
  • 1 Post By vonboett
  • 1 Post By niaz

Reply
 
LinkBack Thread Tools Display Modes
Old   May 5, 2012, 14:59
Default interfoam BC
  #1
Senior Member
 
niaz's Avatar
 
A_R
Join Date: Jun 2009
Posts: 118
Rep Power: 8
niaz is on a distinguished road
Dear Foamers
I want to simulate a single cylinder in 2 phase flow with interface i have tested many conditions but i cannot give regular reason
please help me
my answer and 0/ folder is attached
Attached Images
File Type: jpg alpha.jpg (60.4 KB, 142 views)
Attached Files
File Type: zip 0.zip (3.9 KB, 20 views)
niaz is offline   Reply With Quote

Old   May 5, 2012, 16:51
Default
  #2
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
your problem definition is vague
put the whole case!
at least users can see each boundary condition name where it is!
however it seems you want to model a cylinder one phase is stagnant and the other phase has the velocity of 1 m/s.
first as you use p-rgh, i guess there is no difference between bouyant pressure and zeroGradient
second the answer is some how reasonable, as you put inlet1 fixedvalue zero! there is no input mass for phase 1 so gradually, the phase 1 will leave the domain and the level of phase 1 will be reduced
nimasam is offline   Reply With Quote

Old   May 5, 2012, 23:57
Default
  #3
Senior Member
 
niaz's Avatar
 
A_R
Join Date: Jun 2009
Posts: 118
Rep Power: 8
niaz is on a distinguished road
Dear Nima
thanks for your reply. yes you guess truly.
I send address of my test case. I want to have stable atmosphere on the top of my domain so I use zero as value for inlet. But if you look more carefully, it seems that the second phase mass want to leave the domain like a dam that is broken.
I want to save two phases in my domain.

http://amirms81.persiangig.com/damBreak.zip
niaz is offline   Reply With Quote

Old   June 15, 2012, 05:39
Default
  #4
Senior Member
 
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 178
Rep Power: 6
vonboett is on a distinguished road
Hello A_R, have you tried to switch your outlet and up boundary conditions in the p_rgh file, e. g. buoyantPressure at the outlet and atmosphere type totalPressure at up, together with type inletOutlet; inletValue uniform 0; value uniform 0; for alpha1 at up?

Or, try the following: Move the mesh from positive to the negative x-coordinate quadrant, that has funny influence on the outlet BC!
amin66 likes this.
vonboett is offline   Reply With Quote

Old   June 15, 2012, 15:01
Default
  #5
Senior Member
 
niaz's Avatar
 
A_R
Join Date: Jun 2009
Posts: 118
Rep Power: 8
niaz is on a distinguished road
Quote:
Originally Posted by vonboett View Post
Hello A_R, have you tried to switch your outlet and up boundary conditions in the p_rgh file, e. g. buoyantPressure at the outlet and atmosphere type totalPressure at up, together with type inletOutlet; inletValue uniform 0; value uniform 0; for alpha1 at up?

Or, try the following: Move the mesh from positive to the negative x-coordinate quadrant, that has funny influence on the outlet BC!
thanks, I used correctedFlux and it works fine.
amin66 likes this.
niaz is offline   Reply With Quote

Old   July 2, 2012, 19:07
Default
  #6
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
Quote:
Originally Posted by niaz View Post
thanks, I used correctedFlux and it works fine.
Dear A_R
I'm working in free surface like you, and i have problems with your simulate yet.
i attached my physical domain picture.for example in my case: Re=180, Fr=.6, D=2m
if you can please help

1. what's the BC for alpha, U, P in each boundary? (inlet_air, inlet_water, outlet air, outlet water, up, down, cylinder)

2. you mentioned your simulation became fine, can i know your physical conditions?

3. if you validate your results(Cd, Cl, wave pattern) with any article please inform us.

Regards
Amin
Attached Images
File Type: jpg 2phase.jpg (19.2 KB, 63 views)
amin66 is offline   Reply With Quote

Old   July 3, 2012, 04:13
Default
  #7
Senior Member
 
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 178
Rep Power: 6
vonboett is on a distinguished road
Hi Amin, will you run only 2D cases? I assume you only model laminar flow with Re=180, so you will not have to account for turbulence with free surface flow and complex geometry. A nice discussion about BC can be found here: http://www.cfd-online.com/Forums/ope...interfoam.html
vonboett is offline   Reply With Quote

Old   July 3, 2012, 08:15
Default
  #8
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
Hi Albercht
tnx for your answer. yes, for now i want to simulate 2D,laminar. after obtain good results i have to change my model to turbulent and 3D.
i prefer to use default properties for water and air. with D=2m, rho=1000, nu=10^-6 for Re=180, we should set U=0.00009 m/s. can we use this very low velocity? does it give us reasonable results in OF? also with this velocity Fr will be 2.03*10^-5 so i can't obtain Fr=.6 !!!
How can i balance default properties, Re, Fr? my mean is how can we have favorite Re,Fr and default properties all together? which is more important to set first?

regards

Last edited by amin66; July 3, 2012 at 09:01.
amin66 is offline   Reply With Quote

Old   July 3, 2012, 10:30
Default
  #9
Senior Member
 
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 178
Rep Power: 6
vonboett is on a distinguished road
Hi Amin, I expect you define your Froude number using a characteristic length. How did you define your characteristic length that Fr equals 2.03*10^-5?
vonboett is offline   Reply With Quote

Old   July 3, 2012, 14:30
Default
  #10
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
Hi Albercht
characteristic length is equal to cylinder diameter=2m .
amin66 is offline   Reply With Quote

Old   July 4, 2012, 03:42
Default
  #11
Senior Member
 
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 178
Rep Power: 6
vonboett is on a distinguished road
Well, if you use Fr = v/(gL)^0.5 and Re = vL/nu the ratio between Re and Fr will always be the same independent of the velocity. How were the values of your case defined, at the undisturbed channel or at the cylinder? I would work with a 3D model in a size, defining Re using the hydraulic radius of the channel and definig Fr using the flow depth as characteristic length. You will not be able to increase Fr, but at least you can have higher velocities, for example with depth and width 4m you can get about 0.00016 m/s with Re 187 in the channel. However, is your focus on the discharge of the channel or on the forces at the cilynder? With the mentioned setup, waves will propagate against the flow much faster than with Fr = 0.6 but both are far from critical discharge. If Fr and Re are determined at the cylinder, with flow depth = water depth at cylinder - diameter, the situation is different and you can get higher velocities and Fr for Re 180.

Last edited by vonboett; July 4, 2012 at 05:40.
vonboett is offline   Reply With Quote

Old   July 4, 2012, 07:02
Default
  #12
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
ok tnx, let me to clear my problem:

it's about wave making resistance(wave drag) of a submerged body(2D,3D) as shown in post #6. this bodies for example are under the free surface of sea, but for simulation i think i have to use open channel flow and i think InterFoam is the best for my problem. am i right?

i want to obtain drag force and Cd of this bodies for different submergence depth and Fr numbers. so the Cd is more important to achieve.

i start with laminar for now and then will shift to turbulent model. to calculate Re(Re = vd/nu) and Fr( Fr = v/(gd)^0.5) using the d(cylinder diameter) and properties of water.
amin66 is offline   Reply With Quote

Old   July 5, 2012, 03:36
Default
  #13
Senior Member
 
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 178
Rep Power: 6
vonboett is on a distinguished road
Hi Amin,
I see. InterFoam is good if your body is fixed in its position. But if your body will have the possibility to move due to drag, I strongly recommend interDyMFoam to account for the interaction. If you look at the floatingObject Tutorial, yust be aware what is discussed here.
The floating object tutorial
Since it is about wave drag, I would give higher priority to Fr than to Re, and introduce turbulence as very next step. I think Re can go up to 10^5 allowing the neglection of turbulence in a first step.
vonboett is offline   Reply With Quote

Old   July 5, 2012, 10:45
Default
  #14
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
Hi Albercht
yes my case is fixed. i used other BC and my simulation is better now. i say it's better because the water level don't decrease at outlet as dear A_R said before. now i can see the wave on free surface and vortex shedding behind the cylinder. but unfortunately i dont have any source yet to validate Cd with my results.

guys that work on free surface can look at this article: "Flow past a cylinder close to a free surface" By P. REICHL, K. HOURIGAN AND M.C. THOMPSON

it's helpful but discussed just about wakes.

the BCs taht i used, are similar the new solver (LTSInterfoam) in OF 2. i use OF 1.6 yet!!!

thanks very much for your attentions.
amin66 is offline   Reply With Quote

Old   July 5, 2012, 11:32
Default
  #15
Senior Member
 
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 178
Rep Power: 6
vonboett is on a distinguished road
Hi Amin, cool. What Fr and Re did you use?
vonboett is offline   Reply With Quote

Old   July 5, 2012, 16:47
Default
  #16
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
Albercht, I used u=2 m/s and d=2m ,so fr=0.45 and Re=4*10^6 !!! and it's funny that i used laminar model.

yes i know it's far from reality, but i just wanted to obtain BC for now.
after that i wanted to simulate with Fr=0.6 and Re=180 so i scaled my mesh with gambit to mm, for that mesh diameter became 2mm and i had to use u=.09 m/s to reach Fr=0.6 and Re=180. but unfortunately for every 0.05 pass time my laptop was working about 20min. so i left that till i run with a powerful PC.
i will inform you my result after that.
amin66 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
InterFoam stops after deltaT goes to 1e14 francesco_b OpenFOAM Running, Solving & CFD 8 July 31, 2013 02:29
Segmentation fault in interFoam run through openMPI voingiappone OpenFOAM 16 November 2, 2011 07:49
Slow interFoam compared with other CFD tools? Ralph M OpenFOAM Programming & Development 1 November 17, 2010 07:46
Steady state version of interFoam anger OpenFOAM Running, Solving & CFD 1 October 1, 2009 12:49
Open Channel Flow using InterFoam type solver sxhdhi OpenFOAM Running, Solving & CFD 3 May 5, 2009 21:58


All times are GMT -4. The time now is 22:52.