November 23, 2018 at 2:14 pmcarloruSubscriberI'm trying to simulate a water jet inside a de Laval nozzle. The inlet pressure is equal to 300 MPa, and at the outlet there is air in atmospheric conditions. Inside the nozzle I need to simulate the phase transformation from water to steam due to the low pressure achieved.
I wanted to know what settings are most suitable for this kind of simulation.
Attached the geometric I'm using.
November 23, 2018 at 2:41 pmDrAmineAnsys Employee
So you are expecting cavitation of water in your nozzle as your liquid would experience zones of lower pressures then the vapor pressure. Please look after a cavitation tutorial in ANSYS Flluent created by Raef.
November 23, 2018 at 4:07 pmcarloruSubscriber
Thanks for your answer.
I tried to use the settings that indicates this video but it diverges after a few iterations. I don't know if it's due to the very high pressure inlet.
Also I need to analyze the output of the flow in atmospheric environment, so there is air as third phase.
One of my doubts is whether I have to set water vapor as constant density or as ideal gas.
November 23, 2018 at 4:55 pmDrAmineAnsys Employee
Start with higher Gauge pressure at outlet then Reduce it slowly. You can make both fluid pressure dependent. Compressible liquid for water and ideal gas for water vapor. Switch Energy equation Off at first Stage.
November 23, 2018 at 5:06 pmcarloruSubscriber
I'll try reducing gauge pressure at outlet slowly.
Thank you Amine
November 26, 2018 at 10:20 amcarloruSubscriber
I can't switch energy equation off if the water density is set as compressible liquid and the vapor density is set as ideal gas.
if I set compressible liquid and ideal gas for the densities, even by setting a lower pressure difference, the simulation will diverges immediately.
November 26, 2018 at 1:03 pmDrAmineAnsys Employee
You can switch off the energy equation from "Controls>Equations"
November 26, 2018 at 3:25 pmcarloruSubscriber
I tried to do everything you advised me, but it still doesn't work.
I set the density of water as compressive liquid and the densities of air and water-vapor as ideal gas.
I set the input pressure equal to 2 atm (I would like to be able to do a simulation with an input pressure of 300 MPa).
I have also deactivated the energy equation.
If I imposed the densities as constant the simulation converges, otherwise it doesn't. I cannot understand how to fix this problem.
Attached the fluent case file, maybe it can help
November 26, 2018 at 5:14 pmRobAnsys Employee
As staff we're not allowed to download files, so can only work with posted images. Please can you post some images of the domain (with dimensions), mesh and some results.
November 27, 2018 at 11:31 am
November 28, 2018 at 11:52 amKarthik RAdministrator
Couple of things:
- I'm not quite sure if I have missed it somehow, but I could not see any outlet in your model. Are you modeling the outlet using Pressure Inlet boundary conditions? If so, could you explain why? Also, have to tried pressure outlet in place of pressure inlet?
- It seems to me that your your inlet pressure is orders of magnitude higher than your cavitation pressure. I think Amine is right here. The solution might be diverging because of very high pressure difference. Please try and reduce either your inlet pressure to a small value and incrementally increase this as you the flow stabilizes. Or Increase your outlet pressure value and subsequently reduce your outlet pressure. This should help the flow converge.
- Also, what is your operating pressure? I'd definitely make the operating pressure = 0 Pa and use absolute values of pressures in your model to make sure you are using the right set of parameters.
Please let us know what you find.
November 28, 2018 at 12:16 pmcarloruSubscriber
In the screenshot of the geometry I forgot to write the outlet, but in the simulation there is. The vertical wall on the right is set as pressure outlet, and its gauge pressure is set to 0, as is shown in one of the previous figures.
My operating pressure is actually 101315 Pa. I could set it to 0 Pa in order to use absolute values of pressures but it doesn't change the results.
The simulation's aim is set 300MPa as pressure inlet. I initially set 500000 Pa as pressure inlet and then I will incrementally increase it in order to reach 300 MPa as pressure inlet. I thought a difference in pressure between input and output of 500000 Pa was enough to achieve convergence, but it's not.
I try to lower this difference further, but I wonder how many increments I have to make to reach the pressure inlet at 300 MPa.
The only advice is then to further decrease the inlet pressure? Are the other settings correct?
Thanks for your help,
November 28, 2018 at 1:09 pmDrAmineAnsys Employee
Increase the outlet pressure (use a ramp to lower it back) or increase the inlet pressure (to increase the cavitation number). Use Pseudo transient with small time scale (1e-8
) and start with hybrid initialisation.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Time Step Size and Courant Number
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Floating point exception
- Exporting Data Results