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

Weird hydraulic jump with interFoam [SST k-omega]

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

Like Tree2Likes
  • 1 Post By keepfit
  • 1 Post By Phicau

Reply
 
LinkBack Thread Tools Display Modes
Old   May 7, 2013, 22:23
Default Weird hydraulic jump with interFoam [SST k-omega]
  #1
Member
 
David Long
Join Date: May 2012
Location: Germany
Posts: 55
Rep Power: 5
keepfit is on a distinguished road
Hi Foamers,

I want to simulate free surface flow (or stream flow) around cylinder. Now RAS model SST k-omega is used.



[v=2m/s at +x direction, the water level is set to h=0.6m using groovyBC]


It seems that the results looks reasonable (see Fig above), however, the hydraulic jump at the front of Cylinder looks weird, while the flow is more or less "dynamically stable". Is it because the inlet is too close to the Obstacle - cylinder?



I checked the BCs but could not figure this out, is there some wrong the BCs with inlet?

Best

David
wes1204 likes this.

Last edited by keepfit; May 10, 2013 at 00:01.
keepfit is offline   Reply With Quote

Old   May 8, 2013, 02:39
Default
  #2
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Posts: 237
Rep Power: 7
Phicau is on a distinguished road
Hi David,

you are specifying 2 conditions for the flow: level and velocity.

Your level is increasing due to the presence of the obstacle, but GroovyBC does not allow the flow to reach the boundary (see how there is no water above your given level for the cells adjacent to the inlet).

Depending on what was your goal, taking the inlet far away enough from the cylinder may solve your problem, if you want to prescribe both level and velocity.

If what you need to impose is only a discharge (velocity) I guess you should leave alpha1 as zeroGradient and code a BC to calculate the wet area and apply the calculated velocity to such area. In this case you most probably can reach a stable state with your current domain.

Best,

Pablo
ngj likes this.
Phicau is offline   Reply With Quote

Old   May 8, 2013, 06:09
Default
  #3
Member
 
David Long
Join Date: May 2012
Location: Germany
Posts: 55
Rep Power: 5
keepfit is on a distinguished road
Quote:
Originally Posted by Phicau View Post
Hi David,

you are specifying 2 conditions for the flow: level and velocity.

Your level is increasing due to the presence of the obstacle, but GroovyBC does not allow the flow to reach the boundary (see how there is no water above your given level for the cells adjacent to the inlet).

Depending on what was your goal, taking the inlet far away enough from the cylinder may solve your problem, if you want to prescribe both level and velocity.

If what you need to impose is only a discharge (velocity) I guess you should leave alpha1 as zeroGradient and code a BC to calculate the wet area and apply the calculated velocity to such area. In this case you most probably can reach a stable state with your current domain.

Best,

Pablo


thanks for your tips.

the inlet velocity is set quite low while keep the water level, now the result is fine!

Btw, how to set the outlet BCs to achieve the same water level as inlet's?

best,

David
Attached Images
File Type: jpg sur.jpg (28.0 KB, 268 views)
keepfit is offline   Reply With Quote

Old   November 23, 2013, 13:06
Default
  #4
New Member
 
Baek, Donghae
Join Date: Jan 2013
Location: Seoul
Posts: 24
Rep Power: 4
wes1204 is on a distinguished road
hi keepfit

can i ask BC of your case?

U and p_rgh

I am carrying out the case similar to yours
wes1204 is offline   Reply With Quote

Old   February 17, 2014, 17:22
Default
  #5
New Member
 
Matej Muller
Join Date: Oct 2011
Posts: 8
Rep Power: 5
matejmuller is on a distinguished road
Hi keepfit!

Were you using interFoam or LTSInterFoam for your case? Which fvSolvers and fvSchemes did you use for the kOmegaSST model? I'm trying to run interFoam with the kOmegaSST turbulence model, but I don't know which solvers and schemes to use, since the tutorial for kOmegaSST is only for the LTSInterFoam.

Thanks for the help!
best, Matej
matejmuller is offline   Reply With Quote

Old   February 18, 2014, 22:39
Default Downstream boundary
  #6
New Member
 
Michael Celli
Join Date: Jul 2012
Posts: 2
Rep Power: 0
elephant is on a distinguished road
To answer the question about setting the downstream water level, this can be a bit tricky in OpenFOAM compared to other solvers.

Your current downstream boundary conditions are von neumann (eg. zeroGradient) for pressure, so the boundary isn't influencing upstream pressure in the domain. If you want to influence the upstream water level, you need to set a dirichlet condition using fixedValue or some formula for the hydrostatic pressure at the downstream boundary.

Flow3D accomplishes this with a hydrostatic boundary condition, where an outlet water depth can actually be specified. Within OpenFOAM, I've had success using totalPressure, and setting the value to the water depth * specific weight of the fluid (e.g. 9810 Pa for water). Water depth should match your initial condition for alpha.

The above technique can require some trial and error to prevent sloshing. Also, the above formula only applies to the liquid phase. You will need to apply a neumann boundary or totalPressure of 0 for the air portion of the boundary. Be careful of the phase interface in your implementation.

Once you have it working, I'd be interested to see the results.
elephant is offline   Reply With Quote

Old   March 23, 2015, 13:55
Default
  #7
Member
 
David Long
Join Date: May 2012
Location: Germany
Posts: 55
Rep Power: 5
keepfit is on a distinguished road
Didnt login CFD-Online for a long time since I was working on DEM-CFD couling topic.

I will give a try when i have time.
keepfit is offline   Reply With Quote

Reply

Tags
hydraulic jump, interfoam, sst k-omega

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 | Hydraulic Jump | Correct boundary condition p_rgh pythag0ra5 OpenFOAM Running, Solving & CFD 17 September 5, 2014 04:31
hydraulic jump imanmirzaiian FLUENT 1 February 13, 2014 01:11
hydraulic jump Barry CFX 11 November 24, 2011 17:53
Hydraulic jump The King OpenFOAM 4 November 24, 2011 13:45
Could CFX solve hydraulic jump problem? Andy Chen CFX 0 August 18, 2009 10:13


All times are GMT -4. The time now is 22:27.