Velocity Solution Artefacts

Questions and remarks about code_saturne usage
Forum rules
Please read the forum usage recommendations before posting.
rbecker
Posts: 16
Joined: Thu Jun 28, 2012 4:35 pm

Velocity Solution Artefacts

Post by rbecker »

Hello,

in a very early stage of my CFD I could observe solution artefacts in the z-component of the velocity (the stripes in the solution), Bulk velocity (x-direction) is approx. 30m/s.
Vel-Artefacts.PNG
With ongoing solution process the solution worses and a pronounced pattern in the velocity is visible.
OnGoingSim.png
I've tried the different solution schemes (upwind, centered, solu), different values for pressure relaxation, gradient calculation (Gauss-Seidel, Least Square), pressure gradient extrapolation, blending ... but nothing helps.

Do you have a hint for me how I can avoid this? The grid may not be the best, but is mostly a regular hex cell grid and all quality criterions are fine:

Code: Select all

  Criterion 1: Orthogonality:
    Number of bad cells detected: 0 -->   0 %

  Criterion 2: Offset:
    Number of bad cells detected: 29441 -->   0 %

  Criterion 3: Least-Squares Gradient Quality:
    Number of bad cells detected: 411 -->   0 %

  Criterion 4: Cells Volume Ratio:
    Number of bad cells detected: 0 -->   0 %

  Criterion 5: Guilt by Association:
    Number of bad cells detected: 0 -->   0 %
grid.png
Thank you in advance.

Kind regards,
Ralf Becker
Yvan Fournier
Posts: 4070
Joined: Mon Feb 20, 2012 3:25 pm

Re: Velocity Solution Artefacts

Post by Yvan Fournier »

Hello,

Which version of the code is this ? Could you post a few solver logs ? This might be a CFL/Rhie & Chow filter issue. In any case, logs should help to try to pinpoint the issue.

Best regards,

Yvan
rbecker
Posts: 16
Joined: Thu Jun 28, 2012 4:35 pm

Re: Velocity Solution Artefacts

Post by rbecker »

Dear Yvan,

thank you for the suggestion.

The CFL-Numbers seem to be in a valid range, There are a bit large in the tetrahedral region but shouldn't cause the checkerboard pattern.
Velocity-Z.png
CFl.png
I've attached the XML-file and the logs. CS-Version 6.0.4

Thank you in advance.
Kind regards
Ralf
Attachments
setup.zip
(35.5 KiB) Downloaded 77 times
Yvan Fournier
Posts: 4070
Joined: Mon Feb 20, 2012 3:25 pm

Re: Velocity Solution Artefacts

Post by Yvan Fournier »

Hello,

Did you try "improved pressure interpolation in stratified flow" in the numerical parameters ? This is now the default in v7.0, and may have some influence n cases with buoyancy (it has also been slightly improved in development versions, though I would not expect a significant difference with the v7.0 implementation).

Another option than might have some influence is the "irevmc" (reconstruction of velocity with updated pressure).

Best regards,

Yvan
MaGgo22
Posts: 1
Joined: Wed Aug 17, 2022 3:34 pm

Re: Velocity Solution Artefacts

Post by MaGgo22 »

Dear Ralf,

another test that can be carried out is using a local time step (time- and space varying, 'pseudo-steady') ; starting with a reference time step 'not too small' (for instance 10^(-4)s) - this may contribute to stabilize your results.

Best
Mathieu
Antech
Posts: 197
Joined: Wed Jun 10, 2015 10:02 am

Re: Velocity Solution Artefacts

Post by Antech »

Hello.
I faced similar but not the same problem. Fluid domain is a rapid channel turn with rectangular head loss / heat source region after it (heat exchnger). Velocity level in head loss region is about 1..2 m/s. Although streamlines look reasonable (near straight due to distributed resistance) in some zones velocity drops to very small values and then return back to normal. In a cross-section of resistance region it looks like blue spots on velocity magnitude contour. Switching to first-order discretisation (Upwind) didn't help. In the same zones there is all good in CFX results (although CFX created apparent artifact in another place that is characteristic for it). Pressure field is OK. Density profile is OK.

Saturne version: 7.0.2
Mesh type: tetra without inflation layers
Fluid: Air with variable density
Turbulence: default k-epsilon
Temperature scalar: Temperature Celsius (approx 30...150 *C range in heat exchanger)
Gradient: Least squares + all vertex adjacent
Improved pressure interpolation: On
Time stepping: Local timestep
Reference timestep: 0.0001 s
Target CFL number: 2.0
Local timestep range: 0.00029...0.1 s
Local CFL range: 0.010...8.5

Case XML file, listing and artifact illustration are attached.
Attachments
Artifact in resistance region cross-section
Artifact in resistance region cross-section
run_solver.log
Listing
(1.33 MiB) Downloaded 69 times
A-G000-R000-S000.xml
Case file
(11.97 KiB) Downloaded 63 times
Antech
Posts: 197
Joined: Wed Jun 10, 2015 10:02 am

Re: Velocity Solution Artefacts

Post by Antech »

The problem disappeared after reducing target CFL number from 2.0 to 0.5...1.0 (real local CFL maximum < 2). So it was numerical scheme instability. But, in some cases, there may be instability indeed with lower target CFL numbers, so it's not a universal solution.
Yvan Fournier
Posts: 4070
Joined: Mon Feb 20, 2012 3:25 pm

Re: Velocity Solution Artefacts

Post by Yvan Fournier »

Hello,

Thanks for the feedback. I lnow some colleagues are trying to improve things on this side, but this issue touches on the velocity-pressure coupling and Rhie and Chow filter, where each possible solution has tradeoffs....

In general, we tend to observe divergence of the computation when the CFL becomes too large (though for simple enough cases the slope limiters are sufficient and the computation runs), and checkerboarding when it is too small. When there is a mix of both situations, it is harder to guess how things may behave.

Best regards,

Yvan
Antech
Posts: 197
Joined: Wed Jun 10, 2015 10:02 am

Re: Velocity Solution Artefacts

Post by Antech »

Thanks for you description about CFL numbers. Maybe some extra options in GUI will be useful for cases with such problems.
rbecker
Posts: 16
Joined: Thu Jun 28, 2012 4:35 pm

Re: Velocity Solution Artefacts

Post by rbecker »

Yvan, thank you for the insight and the suggestions.

I've tried several options and CFL-Number choices. As the velocity magnitude in the current setup covers a large span, the CFL-Numbers are either much to large resulting in unphysical solutions or way to small and the checkerboarding occurs. Changing the difference scheme, solver options using the stratified flow options ... does not help.

At least I've found to remedies: either using a pure tetrahedral mesh or switching the turbulence model on the hexahedral mesh off.

Please excuse the delayed response.


Kind regards,
Ralf
Post Reply