April 9, 2020 at 7:14 amconniSubscriber
I am working with an axisymmetric mesh in Fluent created in Workbench Meshing. I built the mesh by using the x-axis as axis and only working in the positive xy-plane. When importing the mesh in Fluent, it correctly assigns the named selections (inlet,outet,wall,axis). When performing a mesh check it fails with a warning saying:
Checking for nodes that lie below the x-axis.
WARNING: Invalid axisymmetric mesh with nodes lying below the x-axis.
Checking element type consistency.
I checked in the Meshing tool, there is nothing below the x-axis. Also, at the beginning of the mesh check, Fluent says:
x-coordinate: min (m) = 0.000000e+00, max (m) = 4.807069e-01
y-coordinate: min (m) = 0.000000e+00, max (m) = 1.875000e-02
Therefore, I do not understand how a node can be below the x axis if the same check that produces this warning says the domain only extends to xmin = 0.0
When I use the TUI command "repair mesh" and check the mesh again, it does not produce this warning. However, I want to understnd how this issue is caused, so I can avoid it without using the repair-mesh function of which I am unsure how it works "in the background".
Any advice is greatly appreciated.
April 9, 2020 at 12:09 pmDrAmineAnsys Employee
One can think that Fluent corrected everything in background but I cannot tell you now what is going on. Please export the mesh and read it in Fluent Standalone outside of the Workbench and check if you get the same issues.
April 9, 2020 at 1:51 pmconniSubscriber
Thank you for the quick reply abenhadj,
as a matter of fact I am running my simulations in standalone Fluent. I only use the Workbench for creating the geometry and mesh. I then export the Mesh as .msh file and import it to the standalone Fluent. Then, the error occurs.
April 9, 2020 at 2:49 pmRobAnsys Employee
In Fluent look in Translate (Domain tab I think). It's probably a rounding error from Meshing and your minimum y value will be -1e-12m or similar. Which version are you using as tolerancing was fixed ages ago. You can then use the Transform option to shift the model slightly "up" so that y>=0
April 10, 2020 at 9:11 amconniSubscriber
Thanks for the suggestion rwoolhou !
I will try it out later and mark the answer as solution if it works. I am using Fluent 2019R3 ,so a pretty up-to-date release i believe.
April 16, 2020 at 6:07 amconniSubscriber
Thanks for the solution rwoolhou,
when clicking on "Transform" --> "Translate" it shows that the domain actually extends to something like negative E-17. I translated the domain into positive y direction by 1.0E-16 and it made the mesh check work (same result as when using "repair mesh").
- 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
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2022 Copyright ANSYS, Inc. All rights reserved.