Water flow through a thick orifice - Non axisymmetric streamlines
I am modeling a thick orifice using a "2D" simulation in CFX.
Inlet BC: Velocity (3 m/s)
Outlet BC: Static pressure, averaged at the outlet.
Details of the Mesh:
Turbulence model: K-e or SST
I am obtaining a non-symmetric streamline at the discharge of the orifice. See the attached pictures:
This is different from what I expected (fig taken from the literature, Roul 2012).
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.
2012. Roul. Numerical Modeling of Pressure drop due to Singlephase Flow of Water and Two-phase Flow of Airwater Mixtures through Thick Orifices.
Your simulation looks like what I would expect, look up the "coanda effect".
Thanks Erik, I learned something new.
Do you think that this phenomenon will exist in flow in pipes?
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.
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.
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).
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
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.
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.
|All times are GMT -4. The time now is 08:30.|