February 1, 2022 at 3:03 pmSardarSubscriber
Consider a mixing tank with its top being open for pressure-outlet BC.
The pressure-outlet window requires backflow turbulence specs.
There is neither inlet, nor downstream/upstream in my case, hence the only statement I found a bit related to my case in the User's guide was: "If the turbulence derives its characteristic length from an obstacle in the flow, such as a perforated plate, it is more appropriate to base the turbulence length scale on the characteristic length of the obstacle rather than on the duct size." which requires to enter the length od he baffle(?) as the length scale. but what about turbulent intensity. I do have an estimation of turbulence intensity in the entire tank but not for the tank top.
Or beyond all these, which "method" should I choose for my case and which values?
ThanksFebruary 1, 2022 at 3:32 pmRobAnsys EmployeeIf you're not including the head space it's more normal to use a symmetry plane at the free surface. If necessary you can put a small vent somewhere out of the way on that surface to let a small amount of material in/out to stabilise the model.
Otherwise you need to find the values at the boundary to avoid messing up the turbulence, species, temperature etc fields.
February 1, 2022 at 5:54 pmSardarSubscriberTogether with what sort of BC can I use a tiny vent? I am patching air on top area of the tank. So should/can I change the pressure outlet BC for tank top to wall BC and then put the vent on the tank top wall? Is that what you mean?
February 2, 2022 at 9:45 amRobAnsys EmployeeIf you have the head space you just need to get the back flow conditions about right: if they're different enough to be effecting the free surface you need to rethink the values.
The vent approach is for when we don't use multiphase and assume the free surface is flat. Depending on the model (material properties etc) we sometimes need a pressure outlet somewhere out of the way to balance the volume in the domain.
February 2, 2022 at 7:56 pmSardarSubscriberI am pretty confused, not making a final answer out of all this post. However, I kind of combined the head space (i.e. air on top part of tank) with symmetry BC and to my surprise, it worked. At least that is how I believe. This is contrary to Rob's first comment, but probably only apparently.
I do not know, maybe I am being a bit pedantic. Any ideas?
February 3, 2022 at 11:15 amRobAnsys EmployeeOK, let's look at the options for modelling.
Liquid (single phase).
Set the top as symmetry and nothing can enter or leave the domain. Assuming no volume is added to the domain it should run nicely. However, a small (1-2 cells) pressure boundary may be necessary to let the pressure stabilise.
Set the top as a pressure boundary. Flow will leave and enter the domain based on the flow field. If extreme vortexing is seen you may empty the tank.
Head space (VOF multiphase)
Set top as symmetry and nothing can enter or leave the domain. You will need good convergence and may need to monitor liquid volume to ensure you aren't gaining or losing mass.
Set the top as a pressure boundary. Flow will leave and enter the domain based on the flow field. If extreme vortexing is seen you may empty the tank, but typically you'll have air recirculating that'll mess with the residuals but won't do much to the liquid flow.
All approaches are valid, and I've used each for projects over the years. Single phase with a pressure boundary is the least stable, and the result is very dependent on the back flow settings.
Viewing 5 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- 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
© 2023 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.