September 13, 2022 at 10:55 amdavide.salvatoreSubscriber
I’m performing external aerodynamics simulations on an ogive-cylinder body in Fluent and I’m facing problems with the generation of “oilflow” pathlines.
The mesh is full hexa, generated in ICEM.
I’m using the k-omega SST model for turbulence and I would like to resolve the viscous sub-layer without wall functions. So, I prepared a low-Re mesh, with a y+<1, which led to a very small value of the first cell height (1e-6, which is 5 order of magnitude less than the length of the body).
The result is that almost all the pathlines get aborted really soon (just dashes), no matter how much I decrease the tolerance.
If I opt for an high-Re mesh, with y+ around 100 and first cell height in the order of 1e-4, the pathlines are computed without problems.
The cells near the wall have good orthogonality, but very stretched (maximum aspect ratio 2e+03), is the high aspect ratio the source of this problem?
September 13, 2022 at 3:27 pmRobAnsys Employee
Aspect ratio may not help, but not sure it ought to break that easily. If you increase the maximum steps do they get any further?
September 13, 2022 at 3:59 pmdavide.salvatoreSubscriber
Hi Rob, thank you for your attention.
Not appreciably. While decreasing the tolerance the number of incomplete paths raise, so I contestually increase the number of steps. The effect is that for increasing number of steps the incomplete paths turn in aborted ones, but the paths remain really short.
September 14, 2022 at 10:57 amRobAnsys Employee
Tolerance should be left alone, it effects the accuracy and default should be good for most cases.
If a pathline is aborted it's becuase you've dropped the tolerance too far https://ansyshelp.ansys.com/account/Secured?returnurl=/Views/Secured/corp/v222/en/flu_ug/flu_ug_sec_discrete_post.html%23x1-159800024.11.2 With default tolerance and 10000 steps how does it look?
September 15, 2022 at 10:20 amdavide.salvatoreSubscriber
If I increase the number of steps (leaving tolerance to default) the effect is that the number of incomplete paths (if any) reduces and the number of aborted increases. Once no incomplete paths are left, all stays the same for increasing number of steps.
For one of the numerous cases I have, setting 10000 steps leads to no inomplete path, and more than 30% aborted paths, even if from the graphic output it seems really that no streamline is completed.
However I have to make a correction: it seems that I was wrong in identifying the first cell height as the critical aspect. I have cases whith small first cell height that show good streamlines, as well as cases with y+ at about 50 that present the problem. Actually I am in the situation in which only old case files showed good streamlines, but of those cases unfortunately I retained only one case file. The strange thing is that the setup doesn’t differ from the new cases of the last 2 months. Even stranger: if I load the new meshes in this case file, initialize and start a computation, the streamlines present no problem, if I start a new case from scratch the streamlines are not computed correctly, same mesh.
Given that behaviour I would like to ask a couple of things:
- Is there a way to know with which version a case file was created? (at the moment I’m using the version 2021R2, it might be that this case file was created with a previous version 2020R2 or even 19.2)
- Do some settings regarding the pathlines plot exist that are not exposed in the GUI, that can affect this behaviour AND that are retained also if I set up a new case from scratch?
Just to be sure: I’m talking about the Pathlines functionality (with oil flow option enabled), not about the Particle Tracking one.
September 15, 2022 at 12:18 pmRobAnsys Employee
Thanks for clarifying, I was looking there. Try doing a DPM plot (just create a dummy injection) and see how that behaves. We switched to "high-res tracking" as default a couple of versions back. It shouldn't matter, but.... I've not seen anyone else report poor behaviour from the oilflow pathlines.
Re the version. The case is (sometimes, depends on zip/format & RAM) human readable and the saved version is there, with .cas it was at the top, you'll need to search for "fluent" in the .cas.h5 format.
September 15, 2022 at 2:50 pmdavide.salvatoreSubscriber
Thank you for the hint. I have searched the .cas.h5 file and two lines result. Pointing in the 2021R2 direction:
(parallel/function "fluent 3ddp -r21.2.0 -ic=default -node -t12")
ANSYS_FLUENT 21.2 Build 10201
Though this file was opened with the 2021R2 version and overwrited from there, so probably this doesn't help that much.
I have tried with particle tracking and it works (as well as the Pathlines plot works if I dont use the oilflow option). Just to be sure that I performed the test you had in mind: I created an injection as a surface, selecting the body surface as source; the particle type I selected was Massless and I left the DPM off.
September 15, 2022 at 3:47 pmRobAnsys Employee
If you do one iteration does the behaviour change? In the TUI type
and press Enter to force an update.
September 15, 2022 at 4:10 pmdavide.salvatoreSubscriber
I don't understand the question, sorry. What behaviour are you referring to? The behaviour of the Pathlines, meaning the way they appear? In that case, which of them? Oilfow or the standard ones?
September 15, 2022 at 4:23 pmRobAnsys Employee
Oil flow pathlines. If something went wrong in the solver an extra iteration can highlight it.
September 15, 2022 at 4:37 pmdavide.salvatoreSubscriber
I will try it tomorrow, now I don’t have access to the files. However for the moment I can say that that is a behaviour that has replicated itself across more than 20 runs, disregarding the mesh, the freestream values and even the solver used (tried with both pressure based and density based).
Moreover today I have tried for the first time to reproduce the same kind of plot with an open source software, exporting the solution data of a case affected by the problem in the Ensight gold format, and they are displayed correctly and qualitatively in line with the expected physics. I honestly don’t know the details of the implementations, but I have tried two approaches:
1. Construct the Wall Shear vector from the exported field values of x_wall_shear,…,z_wall_shear, and plotted the “streamlines” following that vector field, constricted at the surface.
2. Plotted a Line Integral Convolution of the Wall Shear vector field (computed in the same way as point 1).
Both the approaches works. This should rule out a problem in the solver, do you agree?
September 16, 2022 at 10:58 amRobAnsys Employee
Sounds like the post processing for oilflow isn’t working right. It’s been broken before, so it’s possible you’ve found a bug in the function. I’ll raise it.
Edit: Sounds like it's an issue with the oilflow part. All data is good, but the post processing has sporadic issues. Read the release notes in 2023R1 when it comes out.
September 16, 2022 at 3:57 pmdavide.salvatoreSubscriber
The appearance of the pathlines changes within one iteration in a case that should be converged. Moreover the number of aborted lines changes:
at it 1000: number tracked = 1215, aborted = 240, incomplete = 2
at it 1001: number tracked = 1215, aborted = 279, incomplete = 2
I repeat it: judging from the appearance, the pathlines aborted are the totality of them and not “only” 20%~30%.
Thank you for following my case Rob. Please let me know if it results in a bug.
Edit: sorry, I replied to the thread without noticing your edit. So can you confirm that the issue is present also in the 2022 releases?
September 16, 2022 at 4:05 pmRobAnsys Employee
No worries. When you see many abort/incomplete trajectories the numbers tend to vary a little between pathline plots and/or 1-2 iterations.
It may be an issue with 2022Rx, but I can't judge without the case, and that gets messy on here. All I can suggest is reading the 2023R1 release notes: we're also restricted in being able to comment on future releases in any detail....
September 16, 2022 at 4:18 pmdavide.salvatoreSubscriber
I understand. Thank you for your assistance Rob.
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
- 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