# Water flow through a thick orifice - Non axisymmetric streamlines

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 July 24, 2013, 04:47 Water flow through a thick orifice - Non axisymmetric streamlines #1 New Member   Milan Join Date: Nov 2012 Posts: 14 Rep Power: 7 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.

 July 24, 2013, 14:30 #2 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 718 Rep Power: 14 Your simulation looks like what I would expect, look up the "coanda effect".

 July 25, 2013, 17:46 #3 New Member   Milan Join Date: Nov 2012 Posts: 14 Rep Power: 7 Thanks Erik, I learned something new. Do you think that this phenomenon will exist in flow in pipes? Regards Milan

 July 25, 2013, 21:12 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,321 Rep Power: 110 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.

 August 7, 2013, 08:09 #5 New Member   Milan Join Date: Nov 2012 Posts: 14 Rep Power: 7 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

 August 7, 2013, 08:16 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,321 Rep Power: 110 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

 August 7, 2013, 09:23 #7 New Member   Milan Join Date: Nov 2012 Posts: 14 Rep Power: 7 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

 August 7, 2013, 18:28 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,321 Rep Power: 110 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.

 Tags 2d cfx, streamlines pulled down, turbulence models

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Behnam Ghadimi FLUENT 0 June 8, 2013 16:05 kbaker CFX 24 June 14, 2012 07:37 miles_davis OpenFOAM 14 October 11, 2011 17:53 deniggo OpenFOAM Running, Solving & CFD 14 September 30, 2010 03:48 Freeman FLUENT 6 March 4, 2009 03:31

All times are GMT -4. The time now is 12:20.

 Contact Us - CFD Online - Privacy Statement - Top