Pressure instabilities when running RANS on mixed grid type ( Case from DPW7)

[fomistul-cfd]

Hi all, I encounter a problem when running a case for grid convergence from dpw7
The case is :

When inspecting the solution on the surface section the contour plot is showing instabilities that are not influenced by convective scheme , MUSCL reconstruction or limiter.

This was run on a grid generated by me, so to see if it's a grid problem I run also a simulation with comitee grid from dpw7 workshop ( DLR grid with mixed elements)
https://dpw.larc.nasa.gov/DPW7/DLR_Grids.REV00/

When converged the plot showed the same instabilities but on the wing tip where I observed they are appearing on a specific grid topology.
The pressure instabilities:

The grid topology:

We can see that the instabilities appear when a topology of this type is appearing in the grid:

Here is a config file example.

config.txt

I also tried to inspect residuals and orthogonality of the mesh to see if it's a warping/quality problem but the output for quality show zero for all volume cells( it can be me doing something wrong, if someone could help me with that will be great). In term of residuals they were low -8 in logarithmic scale.

Is there something I can do to get rid of these instabilities or is it a bug/ numerical error related problem?

Thank you.

L. E. : In term of force coefficients the results are really good.

[pcarruscag]

Have you tried using Green-Gauss gradient instead of weighted least squares?

[fomistul-cfd]

Hi all , I was a little busy and only now managed to create the cases to highlight the problem on a simple case, it seems that the topology IS the problem. I replicated a flat plate like case in 3D and created 3 cases to calculate, one was tria on surface, one was quad on surface and one was quad with topology modification in the centre of wall surface. Config file was copied from V&V repo for the flat plate. Below we can see the pressure in the middle of the plate. On quad modified we can clearly see the inconsistency of pressure on changed topology. Although in term of value the differences are low, for a case with higher gradient of pressure these are amplified( as is the case from DPW7)

Here is a close-up of the problematic area:

Below are the cases if anyone want to inspect them and run the cases on older versions maybe. Probably I will try it too.
cases.zip

I will also try to triangulate the quad modified case and see if this could solve it.
I hope someone could look into this problem and help solve it.

Thank you.

[bigfooted]

Also shows up with just NAVIER_STOKES as solver...

[bigfooted]

Shows up in energy, pressure and momentum (and density).

[pcarruscag]

Thank you, this is helpful.
Nijso, we have an obscure option to output the dual control volume around a node (in tecplot format I think).
VISUALIZE_CV =
Maybe we find something interesting.

[pcarruscag]

Yeah if you affect pressure or density you affect all conservative quantities.

[bigfooted]

I've made a 2d mesh of a channel flow, here are some pictures:

[bigfooted]

last is pressure

[bigfooted]

control volume seems to be fine:

[bigfooted]

Also happens with INC_NAVIER_STOKES, with rho,T,mu = constant

[pcarruscag]

Since you have hands on, can you test you just free stream, so just uniform moving through a channel with Euler walls, or everything farfield, to see if the mesh preserves the free stream or if there are issues already.

[bigfooted]

Without the wall, so in uniform flow, everything is fine.

[bigfooted]

OK, I thought I was onto something, but paraview also fills the cell differently, depending on the connectivity. This is the reference (moved the cell from the wall to the inner part to rule out a wall effect):

change connectivity of upper trapezoidal cell: (1,2,3,4) -> (2,3,4,1):

It changes the fill color even though the values at the nodes did not change. If you select 'Triangulate' in paraview, the images stay the same.

[bigfooted]

Also happens with INC_EULER (using non-uniform inlet velocity profile), and constant density,temperature

[fomistul-cfd]

Tried to run on older version 7.0.0 and the problem is still showing, on triangulated mesh also the problem is still visible.
Weird that the values are paired( one is a higher and one is lower on inner quad element). Tried to see on my case if the average value is correct if we average all the nodes in the square and compare it with the average without topology modification.

Values are very close so and if we compare the difference with the deviation from expected values procentual is 2.2 %. Probably even with instabilities the solution is conservative. Maybe this could sugest some problem with flux calcualtion or face normals where for one node it's overestimating and other uderestimating?

Line where maximum deviation was taken here, where we know the pressure should be constant.

2D plot of pressure

[pcarruscag]

I think this is just a limitation of the "median dual" approach, if you consider where the dual faces are relative to the middle of the edge (which is where they are considered to be, the "median" in "median dual"), it's pretty impossible to expect perfection.

[fomistul-cfd]

So if this is the problem it seems that only structured grid are suitable for SU2 and unstructured grid will have some percentage of error that could not be quantified?

[pcarruscag]

We will try to improve how we handle the transitions, but I don't think there is a bug in the normals (we check that the dual volumes are water-tight).
I think the smoothness of these transitions is also important. There are other areas with mixed elements in your original image that are fine.
This is an area of the code that was probably not touched since very early on. So hopefully there are easy changes to improve it.

[bigfooted]

Hi @fomistul-cfd , I think this is due to inaccurate flux computations on skewed meshes. Can you share the exact dpw7 grid (.su2 or cgns) and SU2 config file that you used that will reproduce the problem? I will try to see if there are existing solutions for this problem.

[bigfooted]

there has been some work on improving second order accuracy on skewed meshes but it never made it into develop. I ran it on a simple 2d channel case, this is develop vs the improved implementation:


A more realistic case will help figure out if this is worth getting into develop.

[fomistul-cfd]

This definitely looks better, what repo is this? I could run it tomorrow to see how it would work.

[fomistul-cfd]

Hi, @bigfooted this is the link for case that I had been running with tiny DLR grid https://we.tl/t-amfLcWxHl1.

[YairMO]

Hi

Is it possible to share the Channel grid and the accompanying cfg file?

[bigfooted]

Here is the mesh, just replace the filename in your config file. It has markers in,out,wall,sym.
https://drive.google.com/file/d/1t_ElCgt8mW_dCu3oCwFLzNnUWteZMsES/view?usp=sharing

[ErcanUmut60]

I am not sure if its related but I have some sort of instability in the Pressure Inlet Boundary Condition. When I apply time varying pressure at the inlet I get an oscillation at the very first seconds, which can be seen in the graph. SLAU scheme minimizes this error.

Any idea on what might cause this?

[fomistul-cfd]

Maybe first steps are not fully converged, do you start your simulation from an converged steady state? Try to increase inner iterations or lower the time step and see how it would affect the instabilities.

[ErcanUmut60]

I directly start unsteady simulation with MUSCL-on. I don't think it is a convergence issue because I tried those suggestions before and they didn't work.

[fomistul-cfd]

I directly start unsteady simulation with MUSCL-on. I don't think it is a convergence issue because I tried those suggestions before and they didn't work.

Can you try it with pressure not starting from zero? Try making a steady state with ND-Pressure of 0.2, converge it the run your simulation using the steady state as a starting point and see if the oscillations are still present.

[YairMO]

Hi, My apologies, just now I've noticed that the mesh was already attached, sorry. Regards, Yair

…

On Sun, Oct 19, 2025 at 10:05 PM Nijso ***@***.***> wrote: Here is the mesh, just replace the filename in your config file. It has markers in,out,wall,sym. https://drive.google.com/file/d/1t_ElCgt8mW_dCu3oCwFLzNnUWteZMsES/view?usp=sharing — Reply to this email directly, view it on GitHub <#2576 (reply in thread)>, or unsubscribe <https://github.com/notifications/unsubscribe-auth/BJ4NZTLEHYPCPB4SWFIS6CD3YPOHLAVCNFSM6AAAAACHEXR3OCVHI2DSMVQWIX3LMV43URDJONRXK43TNFXW4Q3PNVWWK3TUHMYTINZSGMYTANY> . You are receiving this because you commented.Message ID: ***@***.***>