March 17, 2022 at 8:25 pmjulia.hartigSubscriber
I'm running a transient simulation where backflow occurs periodically through the outlet (a "pressure outflow" BC) due to domain vibration. Since the species fractions near the outlet are time-dependent, there is no appropriate constant mole fraction to set for backflow - at the start of the simulation (i.e t=0s), the backflow condition is most appropriately described by ambient conditions (i.e. n2~0.78, o2~0.22) but as the simulation progresses and product gases reach the outlet, we would expect a more complex stream also containing our byproducts (methane, etc.). I've noticed this is introducing oscillations at the outlet and other unphysical behavior.
I would like to have Fluent assign backflow species concentrations based on the nearest neighboring cell or collection of cells (i.e. closest "downstream" cell) which I should be able to do with a UDF, but I only see options for a constant, parameter-based or expression-based assignment in the species dialog box of the pressure BC. It seems like maybe this would be possible with an expression, since this has a "Locations" dropdown containing my outlet (i.e. 'outlet-top') but I don't know how to reference specific properties/simulation values at this location.
Any advice on how to tackle this issue would be greatly appreciated! I'm leafing through the Users Guide but not seeing any examples relevant to what I'm trying to do so far.March 18, 2022 at 11:20 amRobAnsys EmployeeExpressions ought to do it, but you may need to use the average value from the near boundary region. The facet value on the boundary should include the boundary setting in the calculation so may not be what you want.
March 18, 2022 at 8:11 pmjulia.hartigSubscriberRob Okay that makes sense. I'm really close... but I can't figure out how to make a near-outlet region that will actually appear in the "Locations -> Boundary Zones/Surfaces" dropdown. I created a surface, "outlet_line", but it's not recognized by the expressions utility. If I override it (hardcode the location to "outlet_line") it says that region is invalid.
I guess one way to do this would be to split the outlet tube into two pieces, mesh the interface, and then use that interface as the species averaging location? I hate to do this because it requires reimporting the mesh and redoing the case, and won't be very flexible if I find a better location to extrapolate species fractions from, but maybe this is the only option? What do you think?
March 21, 2022 at 11:52 amRobAnsys EmployeeYou need to split the mesh to get a "proper" surface, but try with a plane too as some of the tools work on those but not iso-surfaces. If the mesh is fairly well aligned near the outlet you can use a register to split the mesh in Fluent. No need to re-mesh.
March 21, 2022 at 4:37 pmjulia.hartigSubscriberI didn't realize you could split the mesh inside Fluent directly, your suggestion is a much easier approach :) Unfortunately the "Surfaces -> New -> Plane" option is greyed out since I'm working in 2D, so I tried splitting with a register. So far it's running without issues, I'll have to see how the results look when it finishes.
March 21, 2022 at 6:43 pmDrAmineAnsys EmployeeUsing udf and providing the t0 value on the face profile.
March 22, 2022 at 5:49 pmjulia.hartigSubscriberThe simulation just finished and the backflow results look good so I think this worked. Thanks for the help Rob! :)
Viewing 6 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
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
© 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.