November 16, 2022 at 7:35 amamkumSubscriber
I am trying to simulate flashing flow of water in CD nozzle in Fluent using Eulerian with thermal phase change model. However, the solution is not converging. I tried changing the scaling factor, still no improvement. Mesh quality is good.
I also tried default cavitation model (Schnerr-Sauer/ Zwart-Gerber-Belamri). In this case convergence is good, but outlet pressure changes to saturation pressure, which is strange (Fig is attched). I have tried both with constant vaporization pressure as well as with UDF. How can this model breach outlet boundary condition, which was imposed?
Thanks in advance!
November 16, 2022 at 8:17 amDrAmineAnsys Employee
I will rather assume equilibirum momentum and use Mixuture Model. Which Nozzle is it? (Paper Reference?)
November 16, 2022 at 8:32 amamkumSubscriber
Thanks a lot for your reply. We have already completed the simulation with mixture model using Zwart-Gerber-Belamri model for mass transfer. Zwart-Gerber-Belamri model for mass transfer hooked as UDF (same UDF crashing with Eulerian model).
Abuaf, N., et al. Study of nonequilibrium flashing of water in a converging-diverging nozzle. Volume 1: experimental. No. NUREG/CR-1864-Vol. 1; BNL-NUREG-51317-Vol. 1. Brookhaven National Lab., Upton, NY (USA), 1981.
We want to improve the accuracy.
November 16, 2022 at 8:42 amDrAmineAnsys Employee
I ran that Abuaf nozzle with Cavitation model and Mixture Model without any UDF and the results are fine. I even used Real Gas Property Tables for that. I think with Thermal Phase Change the key will be to provide a smart heat resistance.
November 17, 2022 at 7:59 amamkumSubscriber
Thanks for your reply.
Are you suggesting using RGP table to give the saturation pressure in the cavitation model?
RGP Table: Lookup in saturation property tables for mass transfer exceeded the lower range 56197 times. Is this treated as error? To generate saturation table, I use the maximum and min pressure value from the previous study of same case. What is the right method to accurately generate this table?
For thermal phase change model, I used the ranz-marshall.
November 17, 2022 at 10:38 amamkumSubscriber
Dear Dr. Amine,
I am simulating BNL309. A screenshot is attached for cavitation model. Please suggest where I am going wrong. When I used UDF with Mixture flow model, the pressure profile was correct. Fluent crashes if I use same UDF with Eulerian model.
However, without UDF, outlet pressure changes to saturation pressure with Zwart-Gerber-Belamri with both mixture and Eulerian model.
November 21, 2022 at 10:16 amDrAmineAnsys Employee
The UDF should be checked if it is crashing with Eulerian Model.
I used RGP tables for Abuaf nozzle and the results were fine. The difference might be that I used expert commands to avoid clipping the pressure as psat. For that reason using UDF for cavitation is also okay. Also bear in mind that Fluent post-processing does limit the pressure to psat when using built-in cavitation model. There is a TUI command to disable that. It is always best to expand the tables with total ranges not only static. The warnings are only printed for static values. I used these limits in my case (again perhaps we are not referring to same case)
I obtained this pressure curve:
November 22, 2022 at 10:16 amamkumSubscriber
Dear Dr. Amine,
Thank you so much for your reply. Now, I can generate the correct RGP table.
But I am still struggling with the cavitation model. I tried setting up the pressure limit by using /solve> set limit. Still, the minimum pressure is clipped to the saturation pressure. Can you please share the TUI command to avoid clipping pressure to psat when using built-in cavitation model? . I tried to find TUI command to disable that. However, I could not find it.
Please help me with this.
November 23, 2022 at 12:17 pmamkumSubscriber
Dear Dr. Amine,
I can resolve the issue which I was facing in the cavitation model. I found the command in Fluent user guide manual.
To see the actual pressure contours, use the following text command:
display clipped pressure in the post-processing [yes]: no
Can you please give some suggestions for thermal phase model. What should be the reasonable value of From Phase Scaling Factor and To Phase Scaling Factor. By default, these are equal to 1.
In some research papers, nozzle pressure, volume fraction, liquid and vapor temperature were initialized with initialization function. Please refer to attached
November 23, 2022 at 12:40 pmDrAmineAnsys Employee
Initialization can assist the steady state solver to quicker convergence without as using Real Fluids + Phase Change might be numerically very stiff.
For the Thermal Phase Change Scalin Factors: they do not exist in Ansys CFX but do exist in Ansys Fluent. I will leave them as default to avoid decoupling the energy balance from mass balance. You can reduce them if you prefer tuning that more than tuning Interfacial Area and HTC alone. I usually do not change that. The referenced paper uses Ansys CFX and so the coefficients are set there to 1.0 You can contact the authors of the paper for more details.
The minimum vapor pressure you can tune is not the one I have in mind (In built in cavitation the material properties are calculated at saturation pressure by default whenever it cavitates -> Incompressible kind of treatment).
- 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
- The solver failed with a non-zero exit code of : 2
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2022 Copyright ANSYS, Inc. All rights reserved.