November 15, 2023 at 10:33 pmIssam EL KHADIRISubscriber
During the simulation the error appears to me
For pressure–velocity coupling, a segregated solver was used with the SIMPLE algorithm. The second-order upwind scheme was used to discretize the convective terms in the governing equations.
The residuals were set to 10−4 for continuity, 10−5 for momentum, and 10−6 for energy equations.
The number of iterations per time step was set to 20.
The time step size 0.001
number of time steps 5000
mesh: 500 000 element
This is the geometry (heat sink TPMS) (Fluid: air, Solid: aluminum)
November 16, 2023 at 3:45 pmRobForum Moderator
What's the mesh quality like?
November 16, 2023 at 10:25 pmIssam EL KHADIRISubscriber
Thank you for your answer,
This is the Report quality:
Minimum Orthogonal Quality = 3.24228e-07 cell 86742 on zone 6 (ID: 1279410 on partition: 2) at location ( 1.00402e-02 7.34195e-03 3.86050e-03)
(To improve Orthogonal quality , use "Inverse Orthogonal Quality" in Fluent Meshing,
where Inverse Orthogonal Quality = 1 - Orthogonal Quality)
Warning: minimum Orthogonal Quality below 0.01.
Maximum Aspect Ratio = 1.34494e+03 cell 296109 on zone 6 (ID: 1115234 on partition: 2) at location ( 5.03466e-02 1.06909e-03 -8.35610e-03)
Fluent can try to improve the mesh quality via the TUI command
x-coordinate: min (m) = -9.000000e-02, max (m) = 1.500000e-01
y-coordinate: min (m) = -1.000664e-02, max (m) = 1.000000e-02
z-coordinate: min (m) = -1.000000e-02, max (m) = 1.050000e-02
minimum volume (m3): 8.992539e-16
maximum volume (m3): 6.769667e-10
total volume (m3): 9.907077e-05
Face area statistics:
minimum face area (m2): 7.985135e-11
maximum face area (m2): 1.673634e-06
November 17, 2023 at 1:13 amIssam EL KHADIRISubscriber
I reduced the mesh to 10 million elements, but the problem persists until now
November 17, 2023 at 9:16 amRobForum Moderator
Yes, it's the mesh. Min ortho quality of 0.05 is considered to be poor quality, you're somewhat below that. Similarly aspect ratio has some leeway for inflation, but 1,300 is very high.
Looking at the second image, check the walls bounding the flow that cut the structure don't have narrow gaps or crevices which then cause the skew cells.
November 17, 2023 at 4:11 pmIssam EL KHADIRISubscriber
I reduced the meshing from half a million to 10 million elements to reduce the effect of meshing
I also checked that the geometry does not have any gaps or crevices.
But no change, the problem still exists
Could the problem be somewhere other than the mesh or the geometry?
November 20, 2023 at 10:48 amRobForum Moderator
And what did that do to the cell quality?
November 23, 2023 at 12:02 amIssam EL KHADIRISubscriber
The problem has been solved. You were right. There was a problem with the mesh.
thank you for your help
November 23, 2023 at 12:12 amIssam EL KHADIRISubscriber
November 23, 2023 at 11:17 amRobForum Moderator
That means you've managed to mesh both zones but not split the solid from the fluid: that may explain the improvement in cell quality.
November 23, 2023 at 11:41 am
November 23, 2023 at 11:44 amRobForum Moderator
Try subtract. Unless you really want to see the solid heat up you don't need it in the CFD model.
November 23, 2023 at 11:47 amIssam EL KHADIRISubscriber
I need to see the heating of the solid with the velocity of the fluid and show the turbulence
November 23, 2023 at 11:49 amRobForum Moderator
OK, so you'll need to subtract and retain the solid and then share topology. The terms etc are covered in the tutorials, and I advise having a look at the various conjugate heat transfer tutorials/videos on the Ansys system.
November 23, 2023 at 12:02 pmIssam EL KHADIRISubscriber
I think that the solid is separated from the fluid because I named each of them in the meshing stage along with naming the boundary conditions/regions. with contact surface
November 23, 2023 at 1:16 pmRobForum Moderator
You've got wall and wall shadow in Fluent and assigned the solid material to the metal part? If you have done that how are the pathlines going through the metal part?
- 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.
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- Suppress Fluent to open with GUI while performing in journal file
- error: Received signal SIGSEGV
© 2023 Copyright ANSYS, Inc. All rights reserved.