February 8, 2022 at 2:04 amjulia.hartigSubscriber
I have a fairly complex simulation (reacting porous media model with dynamic meshing) which has geometry that changes over time as we make improvements to the design. When reading a new mesh, I have not had issues with Fluent's ability to autodetect the inlets and outlets - for example, as long as my pressure outlet is always named "outlet-top", it imports correctly - but the linear periodic boundaries are a constant headache. I have not found any way in ANSYS Meshing/CFD PrepPost to make Fluent able to autodetect a periodic boundary, from creating a Symmetry folder to implementing match controls (seems to fail for 1D boundaries?). I was hoping that as long as I was consistent in my naming convention, Fluent would automatically import a new mesh correctly, but this hasn't seemed to work either. For example, if I have two walls "side1" and "side2" matched as a periodic boundary named "periodic_side1_side2", even if I read back in the *exact same mesh that I created the case with*, it fails to automatically create a periodic zone from side1 and side2. I have quite a lot of interfaces and periodic zones in my model, so this has become very tedious to do manually.
Is there any way around this problem? Am I missing something obvious? Unfortunately my simulation is 2D, so Fluent's Meshing Mode is not an option here.
Thanks!February 8, 2022 at 10:19 amRobAnsys EmployeePeriodics are a little less robust and don't work well with the workflows. In theory match control should help but that assumes a single volume between the two surfaces: in practice that never happens. The better option may be to use the non-conformal periodic (still with very similar cell sizing) and a TUI command to build the periodic interface. Non-conformals that are contact regions in Meshing tend to transfer OK, but check those: the problem is with the wall:## that are created as part of the interface, the numbering doesn't stay the same when a new mesh is read in and that can trigger an error even though the walls don't do anything.
February 8, 2022 at 4:01 pmjulia.hartigSubscriberRob That's too bad. I haven't tried the contact region approach yet because I thought that was reserved for two boundaries at the same location in space (i.e. mine are separated by ~0.15m due to linear periodicity) but I can try that next.
I actually used an edge sizing control with conformal periodics the first time around, which seems to work "ok" meaning no error messages in the console, although not necessarily proof that the BC is being treated appropriately... Is there some reason to prefer nonconformal over conformal here? The dynamic mesh on those boundaries is rigid body translation only (no topology change) so I would think conformal is most suitable.
February 8, 2022 at 4:07 pmRobAnsys EmployeeConformal is better, but assumes you can match the mesh within the tolerance. The contact regions are for touching surfaces, but you can also manually label faces as "interface_whatever" and then set the non-conformal with periodic options. For the latter you may need to switch off the automatic single surface tool, that's covered in the User's Guide on the Interface boundary.
February 8, 2022 at 5:51 pmjulia.hartigSubscriberI see, thank you, this is helpful. I will cross my fingers that ANSYS adds more robust automatic periodic boundary detection in the future :)
February 9, 2022 at 2:42 pmRobAnsys EmployeeIf you keep away from Workbench it may be more reliable. There are tools in/coming in Fluent for solver parameters within the solver so we don't need the external (Workbench) links. Read the 2022R1 release notes.
Viewing 5 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
Ansys BlogTrending discussions
- 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
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- The solver failed with a non-zero exit code of : 2
- Exporting Data Results
- error in cfd post
Top Rated Tags