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

Water flow through a thick orifice - Non axisymmetric streamlines

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 24, 2013, 05:47
Default Water flow through a thick orifice - Non axisymmetric streamlines
  #1
New Member
 
Milan
Join Date: Nov 2012
Posts: 14
Rep Power: 4
milan.2012 is on a distinguished road
Hello

I am modeling a thick orifice using a "2D" simulation in CFX.

Fluid: Water
Inlet BC: Velocity (3 m/s)
Outlet BC: Static pressure, averaged at the outlet.
Details of the Mesh:

Mesh.jpg

Turbulence model: K-e or SST

I am obtaining a non-symmetric streamline at the discharge of the orifice. See the attached pictures:

Streamline_K-e.jpg
Streamline_SST.jpg

This is different from what I expected (fig taken from the literature, Roul 2012).

Expected_streamlines.jpg

The high velocity stream at the discharge of the coefficient is deflected differently (up or down) depending on the turbulence model.

Any suggestions or comments would be greatly appreciated.

BTW no experimental results available.

Milan

References:
2012. Roul. Numerical Modeling of Pressure drop due to Singlephase Flow of Water and Two-phase Flow of Airwater Mixtures through Thick Orifices.
milan.2012 is offline   Reply With Quote

Old   July 24, 2013, 15:30
Default
  #2
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 454
Rep Power: 8
evcelica is on a distinguished road
Your simulation looks like what I would expect, look up the "coanda effect".
evcelica is offline   Reply With Quote

Old   July 25, 2013, 18:46
Default
  #3
New Member
 
Milan
Join Date: Nov 2012
Posts: 14
Rep Power: 4
milan.2012 is on a distinguished road
Thanks Erik, I learned something new.

Do you think that this phenomenon will exist in flow in pipes?

Regards

Milan
milan.2012 is offline   Reply With Quote

Old   July 25, 2013, 22:12
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,758
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Absolutely! It is a general fluid mechanics phenomenon. A fluid jet near a wall will bend and attach itself to the wall. The physics of why it does it is interesting, well worth reading up about.
ghorrocks is offline   Reply With Quote

Old   August 7, 2013, 09:09
Default
  #5
New Member
 
Milan
Join Date: Nov 2012
Posts: 14
Rep Power: 4
milan.2012 is on a distinguished road
Hello again

An update on my problem. I am now doing the simulation with air ideal gas, Inlet BC= normal speed 2.5 m/s, Outlet BC= static pressure 8.35 barg. See below the streamlines for the 3D and 2D simulation, The Coanda effect is not present in the 3D simulation.

Streamlines_3D.jpg
Streamlines_2D.jpg

Has it maybe something to do with the number of elements that I am using?, type of simulation (maybe transient is better than steady state?).

The pressure drop calculated with the 2D simulation is significantly smaller (0.02 bar) than the one calculated with the 3D simulation (2.2 bar, in the order of magnitude of experiments).

Regards
milan.2012 is offline   Reply With Quote

Old   August 7, 2013, 09:16
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,758
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Make sure you are taking into account the thickness of the 2D model when you compare the flowrates.

Your 2D model is artificially constraining the simualtion so it does nto surprise me that it is inaccurate.

The general question on accuracy is an FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   August 7, 2013, 10:23
Default
  #7
New Member
 
Milan
Join Date: Nov 2012
Posts: 14
Rep Power: 4
milan.2012 is on a distinguished road
Hello Glenn, thank you for your prompt answer.

The physical problem that I am trying to solve is similar to the 3D geometry shown in the figure. I have inlet and outlet pressures, fluid type (air), inlet temperature, and mass flow. I calculated the inlet normal velocity with the air density at the inlet and the pipe area.

Your comment: "Make sure you are taking into account the thickness of the 2D model when you compare the flowrates."

I am comparing directly the pressure drop from the 2D and 3D simulation against the experimental value. The results of the 3D simulation give a better match against the experimental data, the 2D simulation is far off.

Your comment: "Your 2D model is artificially constraining the simualtion so it does nto surprise me that it is inaccurate."

Could you expand a bit more on that?. For pipes (or essentially any device with axisymmetry) and single phase flow I thought it was "standard" practice to simulate either a wedge or a plane with a height equal to the pipe diameter.

In this case I would suspect that the difference between the 2D and 3D simulation might be caused by the artificial boundary symmetry condition, that is not capturing what happens in reality in the flow.

Thank you for the webpage about accuracy, it is a nice summary (check list) to take into consideration.

Regards
milan.2012 is offline   Reply With Quote

Old   August 7, 2013, 19:28
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,758
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You have drawn your 2D flow with a thickness. Just make sure you include the thickness in mass flow/volume flow rate calculations.

2D artificially constrains the flow because it does not allow the flow to move in the Z direction. If the flow is naturally 2D anyway (which low and high Re flows usually are) that is not a problem, but for intermediate Re flows you often get flow oscillations in the Z direction which need to be captured if you want to be accurate. So modelling an intermediate Re flow as 2D would cause inaccuracy.
ghorrocks is offline   Reply With Quote

Reply

Tags
2d cfx, streamlines pulled down, turbulence models

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
Mass Flow rate in spray water modeling Behnam Ghadimi FLUENT 0 June 8, 2013 17:05
Discontinuity at water level in stratified 2 phase flow kbaker CFX 24 June 14, 2012 08:37
problem with two phase flow (air injected in water) miles_davis OpenFOAM 14 October 11, 2011 18:53
pressure distribution in water flow, differences in icoFoam and COMSOL deniggo OpenFOAM Running, Solving & CFD 14 September 30, 2010 04:48
Easy question: how to simulate water flow? Freeman FLUENT 6 March 4, 2009 03:31


All times are GMT -4. The time now is 09:54.