search

su2code / SU2

SU2: An Open-Source Suite for Multiphysics Simulation and Design
https://su2code.github.io
Other
1.34k stars 845 forks source link

Strange values at symmetric BC when AXISYMMETRIC=YES #1373

Closed mskim0401 closed 2 months ago

mskim0401 commented 3 years ago

Dear all,

I simulated Sym_plane_testcases from #657 When I simulate axisymmetric probem (AXISYMMETRIC =YES), I found odd value at symmetric axis. This problem doesn't appear when I turn off AXISYMMETRIC option.

Cp_comparison

======================================================================== . .

Density_comparison

======================================================================== . .

Mach_comparison

======================================================================== . .

Temp_comparison

It seems that temperature, Mach, and momentum have no problem, but density, pressure, and energy are strange at the symmetric axis... From #657 , I think it is flux related problem.

I attached version 7 configure file I used. Sym_BC_test.zip

I'm also trying to simulate my axisymmetric problem and this problem appears too in my case. Base_Axis Symmetric BC is x-axis.

How I fix this problem? Could anyone help me?

Thank you.

Desktop (please complete the following information):

pcarruscag commented 3 years ago

Some issues were fixes is version 7.2.0 related with axisymmetry. Give it a try please.

pcarruscag commented 3 years ago

Correction, they were fixed in the develop branch, not released yet #1366

mskim0401 commented 3 years ago

I tried to fix this problem about 10 days. I conducted code in #1366 but there still are problem at near axis. (In my experience, this bug affect not that big effect on solution)

One thing I found is that it can be improved by using Upwind scheme (e.g Roe, HLLC) but not exactly resolved.

I attached density profile using Roe scheme.

![Density](https://user-images.githubusercontent.com/74228020/135422230-5193ca99-a58a-454a-b4d3-b62a6da5b44b.png)
bigfooted commented 3 years ago

I just ran the case and I see this as well, even after complete convergence. You clearly can see this in the energy and pressure (and density) but not in the momentum terms. The temperature field also looks smooth. So may be related to density/pressure.

mskim0401 commented 3 years ago

What I found is that density unrelated values look smooth for example, velocities (I got it Momentum/Density) and total energy (Energy/Density).

As I understand, pressure is calculated assuming perfect gas: image and temperature is image Pressure is function of density but temperature is not. I guess that's why temperature looks good.

However, I don't know why momentum has no problem.

WallyMaier commented 3 years ago

I wonder if this issue arises only with AXISYMMETRIC = YES and a BC_SYM?

mskim0401 commented 3 years ago

I just tested some boundary conditions on O cylinder case. And I found this issue occurs at near axis when AXISYMMETRIC = YES regardless of which BC is applied at axis (y=0). For example, this also arises on BC_HeatFlux_Wall with zero heat flux.

pcarruscag commented 3 years ago

Have you tried different gradient methods? Green-Gauss v Weighted Least Squares

mskim0401 commented 3 years ago

Yes I tried both, however this issue still arose...

jtneedels commented 3 years ago

I'm seeing similar results, even with changing to the compressible solver. I'm noticing that the oscillations, atleast for my case, follow the grid lines near the body. I'm trying to see if turning off portions of the viscous source residual address helps, to try and isolate the problem, but haven't had much luck yet. I'm seeing the problem consistently regardless of limiter choice.

image

WallyMaier commented 3 years ago

@mskim0401 @pcarruscag This problem is seems to even in 2D simulations, when zooming into other blunt-body type cases in NEMO and Flow solver, the same pattern can be seen, just not as significant. It may be a case of axisymmetric making problem worse.

mskim0401 commented 3 years ago

At least for my case, this problem doesn't have a significant impact on the entire solution. In addition, this oscillating pattern appears about only 4 cells near axis regardless of how far it is from the axis.

jtneedels commented 3 years ago

@mskim0401 Yes, that is consistent with what we are seeing. Although the effect seems localized, it is disrupting the solution quality (particularly surface pressure and density) in the vicinity of the stagnation point. @WallyMaier and I are taking a look to isolate the cause.

jtneedels commented 3 years ago

@pcarruscag @mskim0401 @WallyMaier @bigfooted I see these oscillations persistently in non-axisym cases with MUSCL turned off. I went through the BC_SYM_PLANE implementation in CFVMFlowSolverBase.inl, but I couldn't find anything that affects this issue. It's interesting we've observed it in a variety of solvers, could it be how the node at the corner of the symm plane and wall is treated?

ChristianBauerEng commented 2 years ago

Not sure if this issue is related, but I'm performing axisymmetric simulations of a convergent nozzle. Throughout most of the domain the axis values seem fine, but there is a region where density behaves quite strangely at the axis.

What is seen here is the density gradient, just to make it more visible: grafik

Results obtained with SLAU2, 2nd order euler.

pcarruscag commented 2 years ago

Trying to leave something other than the usual "go away stale bot", one theory from the last dev meeting is that the gradients used in the axisymmetric source may need some treatment consistent with the symmetry boundary.

antares190 commented 1 year ago

Just my 2¢ here. I've been struggling with a relatively simple simulation, Euler, 2D axisymmetric, supersonic, AUSM (SU2 7.5.1). I tried several meshes (and meshers) and always diverged no matter what (quality is ok, CFL as well). Conditions were ok, and were mimicking inv_wedge tutorial (which, btw was running ok even with axisymmetry ON).

Long story short, I opened with a text editor the original geometry STEP file, and noticed it was carrying from the CAD some (engineering wise negligible) numerical terms (say, point 0, 0 was actually 0, 1e-6). Hence the symmetry axis was somewhat off. By correcting the STEP file, everything went fine.

I wonder whether this is the expected behavior of this kind of simulation, and / or if there is any artificial diffusion parameter (such as ENTROPY_FIX_COEFF) that actually can sort things out for the EULER mode.

Did any of you experienced anything similar?

Thanks!

pcarruscag commented 1 year ago

Axisymmetry on a node-based code requires special treatment near the axis because some terms are 1/r and so if r is close to zero... If your geometry had the axis at 1e-6 the "axis treatment" was not being applied.

antares190 commented 1 year ago

Thank you Pedro for the lightning reply! Yes, I see, unfortunately, I can't cross-check the log right now to see whether the "STRAIGHT EDGE" string was triggered, but I'll pay attention to that in the future for sure.

Anyway, I wonder whether the axis treatment is looking for a "numerical 0", or does perform some sort of filtering or tolerance on the mesh ( in some ways similar to what some CADs do).

In my case, the body was in the order of meters, and the domain was in the order of 100 m.

bigfooted commented 1 year ago

ANSYS Fluent for instance has the same strict criterion, the axisymmetric line should be placed at the x-axis with high precision. In SU2, y < 1.0e-16 for the y-coordinates of the nodes on the symmetry axis