October 12, 2020 at 1:46 pmramkallSubscriber
I am trying to simulate a 3D liquid receiver tank filled with R134a when the entering flow is 5K subcooled assuming that the tank is at the saturated state initially. the geometry and initial volume fractions are attached. The goal is to see the state of the fluid at the tank outlet in steady-state conditions and also to see the equilibrium level, i.e if the tank is filled and the exit reaches the same inlet temperature or the tank maintain an equilibrium level with a temperature between the inlet and the saturated temperatures.October 12, 2020 at 3:56 pmRobAnsys EmployeeDepending on settings you may need to account for the static head of liquid, so the outlet pressure may be too low. What temperature is the system relative to the boiling point? Again, if boiling occurs too quickly the gas has to go somewhere. What time step are you using?
October 12, 2020 at 5:02 pmramkallSubscriberThanks for your comment static head is accounted using operating density set to zero.
the initial temperature of the gas is at saturated temperature and the inlet liquid is 5K subcooled.
In fact, I used polynomial density of gas via temperature, and apparently as the liquid comes in, the density is constant and so pressure goes up since gas was like incompressible liquid!
I am using Peng-Robinson density for gas now, and mass flow outlet BC instead of pressure outlet. I had a strange pressure changes at the very small times steps at the beginning but it becomes physical now using larger times steps (0.01 s).
The simulation is running to see if I will have a physical volume fraction and temperature or not. I will update it here the possible problems of the model. Like now I can see that the liquid temperature is developing a strange colder column from outlet into the fluid that seems strange.
I highly appreciate if the topic is followed after the update.
October 13, 2020 at 3:33 pmramkallSubscriberDear I tried both pressure outlet and mass flow outlet BCs.
Mass flow outlet: the pressure in the tank goes up to unphysically high values
Pressure outlet: the outlet mass flow rate becomes positive and almost 10 times more than the inlet flow. Also the form of the VF contour seems strange and unphysical. please find it below after some time steps (TS = 0.01 s)
P.S: I set one mass trasnfer mechanism (evaporation-condensation) to model both evaporation and condensation in the tank to find the equilibrium state. I found in the User guide that "From" must be the liquid and "To" must be the gas phase so I assume one mass transfer mechanism can model both evaporation and condensation at the interface.
Please let me know for any tips!
Thank you in advance, best regards.
October 13, 2020 at 3:37 pmRobAnsys EmployeeYou're correct re the mass transfer. I'd use Ideal Gas over the Real Gas options as it tends to be more stable. If the first time steps are odd, what temperature did you patch the gas at? If it's already sub cooled the first thing it'll try and do is contract & condense.
October 13, 2020 at 3:51 pmramkallSubscriberThanks for the comment
I can try ideal gas too.
both gas and liquid are patched at a temperature almost equal to the saturation temperature. gas a bit higher and liquid a bit lower to avoid spontaneous condensaton/evaporation. So the initial state of the tank is saturated and the inlet liquid is 5K subcooled.
What is the contract & condense that I should do?
October 14, 2020 at 10:59 amRobAnsys EmployeeWhat pressure did you patch at? With a compressible gas if you don't get the initial conditions right it'll try and expand/contract to suit the conditions. If you run your model on does the system stabilise and start to drain?
October 15, 2020 at 10:57 amramkallSubscriberThank you very much Rob It is patched at 5 bar and the initial temperature of the tank is equal to the saturation temperature at this pressure (288.8 K). The inlet fluid is at 283.8 K accordingly (5k sub-cooled)
I have tried to outlet BC and different results, both wrong: pressure outlet: pressure in the tank is decreased a bit that seems normal due to pressure of the liquid column, so in the tank must be a bit less that the outlet pressure (5 bar). BUT the outlet mass flow is positive and much higher than the inlet flow! Mass flow outlet: set equal to inlet mass flow, but the pressure goes up to very high values. Maybe VOF should be tried using default tuning coefficients. I tried it before and at least the volume fraction contour was more physical than Eulerian model. but the same high pressure/outlet mass flow was observed with VOF as well! There is no other BC that can be tried I dont know why the models are failed like this.
October 16, 2020 at 11:10 amRobAnsys EmployeeDid you calculate the properties at 5 bar gauge or 5 bar absolute? What's the operating pressure in your model?
October 16, 2020 at 11:38 amramkallSubscriberThanks Rob I calculated them at 5 bar absolute. operating pressure is 1 bar as default. could it be the problem?!October 16, 2020 at 2:00 pmRobAnsys EmployeeProbably, you'll be 1 bar out on the saturation temperature: you're running the model at 6 bar absolute if you've not changed the operating pressure.
October 27, 2020 at 1:17 pmramkallSubscriberThank you Rob To conclude, the problem was as you correctly said the operating pressure. I set it to zero and the simulation becomes physical now.Viewing 11 reply threads
Ansys Innovation Space
- 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.Trending discussions
- 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
Top Rated Tags
© 2022 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.