TAGGED: 2D, 6-dof, dynamic-mesh, negative-volume-detected, rigid-body-dynamics
February 18, 2021 at 4:23 pmpgalvesSubscriber
I have a simple 2D problem of a pipe in which a sphere is placed in the middle (see figure). I want to simulate the motion of the sphere due to the fluid flowing through the pipe. The pipe has 1 inlet in which the velocity is prescribed as 0.30 m/s and 1 outlet where the pressure gauge is set to 0. The flow is laminar. The sphere has a 0.5 mm diameter, which gives a 6.54e-11 m3 in volume. Since the sphere material has a density of 5200 kg/m3, that gives a mass of 3.40e-7 kg.February 18, 2021 at 4:46 pmYasserSelimaSubscriberFirst, as this is 2D problem, Fluent recognizes the sphere as a cylinder. Unfortunately you need to do 3D simulation for this case.nSecond, the drag force is proportional to the fluid density. This means the force in the case of water is almost 800 times that in case of air assuming same velocity.nThird, 20 iterations per time step is not enough. If the flow does not converge, the values of the drag and lift force could be extremely high. This would result in higher particle velocity leading to negative volume cells.nFourth, it seems something is wrong with your remseshing criteria. Can you show the pannel of remeshing as well as your mesh statistics.nFebruary 18, 2021 at 4:48 pmYasserSelimaSubscriberOne more thing to add, you might have separation around the sphere as well. Use transition turbulent modelnFebruary 18, 2021 at 5:34 pmpgalvesSubscriberThank you for your quick answers, Array!nI just have some questions about two points you make:n1): I understand that fluent will interpret the circle as a cylinder and not a sphere, but would that impact its motion in 2D? What I mean is, if the depth is very small, the slice from the middle of a sphere and the slice from a cylinder would be similar/same, no?n4) Which criteria would you think could be wrong? I don't understand what you mean by panel of remeshing. I even posted the smoothing and remeshing settings in duplicate, without noticing it! Regarding the mesh statistics, please check the attached pic:nnThanks for the other suggestions, I will look into it!nFebruary 18, 2021 at 6:08 pmYasserSelimaSubscriber1) The drag coefficient on a sphere is different than that on a cylinder.n2) Sorry my bad, I looked at the mesh but not the panels. Make the minimum length scale zero. Also press on mesh scale info button and post a screenshot Now I believe these cells are coming from the sizing function. Your sizing function makes the new mesh sizes similar to the smallest one. And the change is linear .. so, all remeshed cells becomes very small. Put a positive number in variation and rate .. say 0.1. Or disable the resizing functionFebruary 18, 2021 at 7:59 pmpgalvesSubscriberThank you nHere's a screenshot of the mesh scale info. nRegarding the sizing function, I intended the change to be linear and the remeshed cells to remain small, and did not want to have large cells away from moving circle. You think this is bad? Why?Thank you again for the discussion.nBest regardsnFebruary 18, 2021 at 11:56 pmYasserSelimaSubscriberYou ask Fluent to create mesh that is finer than the original ones.nMake the minimum length scale 0, the max 0.07 or so ... and the skewedness 0.49, similar to the original mesh .nsizing function, put small positive numbers and trynViewing 6 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
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error: Received signal SIGSEGV
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.