When to activate the "Cavitation" option?

nikesh · July 28, 2014, 04:03

Hello...
For my valve flow simulations, when do I enable or activate the cavitation option?
I am simulating ball valves at 10% open interval each. First case 100% full open...I can assume cavitation won't occur, then 90% case, and 80% and so on....but when and how do I know that I have to activate the cavitation option??
Thanks in advance!
Nikesh.

Boris_M · July 29, 2014, 05:53

Hi Nikesh,

a clear indicator is if you see an error message in the solver that you have negative pressure.
Pressure can decrease under the environment pressure (1atm) without cavitation as the pressure has to fall under the saturated vapor pressure for the water to basically evaporate. That point is along a curve of a graph of pressure and temperature. So it depends on the temperature as well. If you consider a isothermal case (temperature does not change), which can be considered in most cases except if you have a heat source and the water is heated in some way, you can use the isothermal cavitation capability of FloEFD. Simply setup a new liquid for water with cavitation option enabled and use the parameter of the original water (you can also copy/paste the original water into the user defined section and change it). Then set cavitation with the molar mass of 0,018 kg/mol, your temperature you consider (it will give an error if that is differently defined in any boundary condition) and the saturation pressure.
And that saturation pressure is also the local pressure at which cavitation can appear if it is equal or below that value.
So defining a minimum global pressure goal can tell you how close you are to cavitation at a certain water temperature.

I hopw this helps,
Boris

Boris

nikesh · August 19, 2014, 22:49

Boris,
I did the same thing you mentioned for my case. I encountered some warnings and here's my case:
Ball valve 60deg closed case.
Inlet BC: Normal to face Inlet Velocity 2 m/s, "Fully developed Flow" enabled
Outlet BC: Static pressure 101325 Pa.
Computational Domain: 20D upstream of valve, 60D downstream
Computational Mesh: Automatic level 5, No of refinement 2
Operating Fluid: water

(FYI: This is a different case which I have adopted from a paper which contains the experimental results with which I want to test my CFD results. Its not the one with Sludge and water)

First, I ran my simulation without the cavitation. This is what I got, but got no warnings in the end (Fig 1 and 2). I'm not sure if there were any warnings during the simulation since I had just left it running over the weekend and came back to check on it only on Monday.
I noticed negative pressure there, (which is less than saturation pressure 2339Pa for water at 20deg C) hence I enabled the cavitation option.
I created a new liquid-gave it a different name, copied the properties of water and clicked on "cavitation". There I changed the molar mass to 0.018 kg/mol and the temperature to 293.2K (same as in the BCs) and the saturation pressure to 2339 Pa (this I obtained from a paper).
Then I started the simulation again and after refinement twice, I got these warnings. Check Fig 3 and 4. These warnings were not present before the 2nd refinement.
Fig5 is the cross section of the part of the valve model.
The result is getting very unrealistic. Let me know if you can make something out of it!
Thanks.
Nikesh.

Boris_M · August 21, 2014, 10:07

Hi Nikesh,

the error message suggest that you have very high flow rate in a very small portion of your fluid volume dV/V suggests it is tiny compared to the overall fluid volume. Usually when this occurs it is in a partial cell. This part of the cell is not very ideal and you can find it by loading the results of this calculation when this message comes and have a look at the min/max values. If the solver crashes because the values soar to infinity then often you still get a r_abnorm.fld result file in the project folder. Load that result and display the global min/max values. You will see a red and blue small sphere in your model. If you don't see one simply create a cut plot and as soon as you have a visualization parameter due to an active plot the min/max will show the min and max value of that parameter. If you change it to velocity you will see the sphere's locations for min and max velicity. Now move the cut plot to the position of the red sphere and deactivate the interpolation and activate the mesh in the cut plot. If the cut plot cuts about right through the sphere you will see one fluid part of a partial cell is fully red and the other cells around it are blue. The value is very local but can silightly "infect" others over time so that it spreads a little. But this one tiny cell is causing the problem.
The easiest way is to move the cell by shifting the whole mesh a little. You can do that by deactivating the automatic mesh settings and go to the basic mesh definition where you can define how many cells are in x, y and z direction. Now simply add one cell in either one of the directions. That will shift the cell slighly and since this phenomena appears very seldom it is most likely gone now. If it still exist, try another direction.

That should solve your problem,
Boris

July 28, 2014, 04:03	When to activate the "Cavitation" option?	#1
nikesh Member Nikesh Bhattarai Join Date: Nov 2011 Location: Sacheon, South Korea Posts: 82 Rep Power: 13	Hello... For my valve flow simulations, when do I enable or activate the cavitation option? I am simulating ball valves at 10% open interval each. First case 100% full open...I can assume cavitation won't occur, then 90% case, and 80% and so on....but when and how do I know that I have to activate the cavitation option?? Thanks in advance! Nikesh.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
sliding mesh problem in CFX	Saima	CFX	46	September 11, 2021 07:38
mass flow in is not equal to mass flow out	saii	CFX	12	March 19, 2018 05:21
Low Mixing time Problem	Mavier	CFX	5	April 29, 2013 00:00
Error finding variable "THERMX"	sunilpatil	CFX	8	April 26, 2013 07:00
Water subcooled boiling	Attesz	CFX	7	January 5, 2013 03:32

July 29, 2014, 05:53		#2
Boris_M Disabled Join Date: Jul 2009 Posts: 616 Rep Power: 23	Hi Nikesh, a clear indicator is if you see an error message in the solver that you have negative pressure. Pressure can decrease under the environment pressure (1atm) without cavitation as the pressure has to fall under the saturated vapor pressure for the water to basically evaporate. That point is along a curve of a graph of pressure and temperature. So it depends on the temperature as well. If you consider a isothermal case (temperature does not change), which can be considered in most cases except if you have a heat source and the water is heated in some way, you can use the isothermal cavitation capability of FloEFD. Simply setup a new liquid for water with cavitation option enabled and use the parameter of the original water (you can also copy/paste the original water into the user defined section and change it). Then set cavitation with the molar mass of 0,018 kg/mol, your temperature you consider (it will give an error if that is differently defined in any boundary condition) and the saturation pressure. And that saturation pressure is also the local pressure at which cavitation can appear if it is equal or below that value. So defining a minimum global pressure goal can tell you how close you are to cavitation at a certain water temperature. I hopw this helps, Boris Boris

August 21, 2014, 10:07		#4
Boris_M Disabled Join Date: Jul 2009 Posts: 616 Rep Power: 23	Hi Nikesh, the error message suggest that you have very high flow rate in a very small portion of your fluid volume dV/V suggests it is tiny compared to the overall fluid volume. Usually when this occurs it is in a partial cell. This part of the cell is not very ideal and you can find it by loading the results of this calculation when this message comes and have a look at the min/max values. If the solver crashes because the values soar to infinity then often you still get a r_abnorm.fld result file in the project folder. Load that result and display the global min/max values. You will see a red and blue small sphere in your model. If you don't see one simply create a cut plot and as soon as you have a visualization parameter due to an active plot the min/max will show the min and max value of that parameter. If you change it to velocity you will see the sphere's locations for min and max velicity. Now move the cut plot to the position of the red sphere and deactivate the interpolation and activate the mesh in the cut plot. If the cut plot cuts about right through the sphere you will see one fluid part of a partial cell is fully red and the other cells around it are blue. The value is very local but can silightly "infect" others over time so that it spreads a little. But this one tiny cell is causing the problem. The easiest way is to move the cell by shifting the whole mesh a little. You can do that by deactivating the automatic mesh settings and go to the basic mesh definition where you can define how many cells are in x, y and z direction. Now simply add one cell in either one of the directions. That will shift the cell slighly and since this phenomena appears very seldom it is most likely gone now. If it still exist, try another direction. That should solve your problem, Boris