[Captain Convergence]

I am facing serious issues with the convergence of my 2D hypersonic case. I gave up trying to perform a full-multigrid intiliazation because it diverges at the back part of my body (the pressure was prone to go below 0 Pa in that region). Therefore I switched to a hybrid initialization. My case is pretty "simple", it is a 2D section of a blunt delta and the free stream conditions are:

Mach 9.6
Temperature 47.18 Kelvin
Pstatic 141.36 Pa
Operating Conditions 0 Pa

I have double checked them with a NASA report of an experiment carried out at the same wind tunnel and they match for the same Mach Number.

At the moment I am performing an inviscid simulation with ideal-gas formulation and pressure far field and symmetries as boundary conditions. However I am experiencing divergence issues because the pressure drops at local points (specially at the symmetry) and this makes the velocity to build up dramatically. I consider that I am using the right solver controls for starting the calculations and ensuring the convergence but correct me if I am wrong:

Density based solver in explicit mode (theoretically more robust than implicit)
Courant number = 0.05
High order terms under-relaxation factor =0.05 (applied to all variables)
Algebraic multigrid with 5 levels in V cycle (rest of setting left by default)

I have attached images of the used mesh. I enabled the MG verbosity (see attached images) and I am suspecting that the solver doesn´t visit the coarser levels of the multigrid because in the console the residuals are not displayed at any level, it only displays ->1.->2.->3.->4.->5.<.....<.....<.....<.....<.... with dots where the residuals should be displayed. However this shouldn´t be the source of the divergence but an indication that I am not setting up the solver properly.

Is there any solver control that I should look at? Thank you in advance!

[vinerm]

Your bluff body is very close to the entrance. That could cause issues. Could you share the link or the paper that you are referring to?

What's your mesh count? Could you share the mesh file, or better, dimensions of the bluff body?

[Captain Convergence]

The paper that I am referring to is this one:

https://ntrs.nasa.gov/search.jsp?R=1...atchallpartial

On the second paragraph page 19 (21 at the PDF), it mentions the free stream conditions that are being assumed.

My mesh has 506K elements (2D), I cannot upload it here because it is 17 megabytes, which is over the upload limit. I have attached an image with the dimensions of the bluff body, it is non-dimensionalized with the thickness t (0.75 in/19.05 mm) therefore the model is 115.062 mm long with a 70 deg sweep.

I am positioning the body that close to the entrance because the propagations will not travel upstream. I almost managed to get a fairly good FMG initialization (see the attached image) and the issue was not at the front, it was at the back because behind the base area the presure is very very low and the CFD solver converges to a negative value which is completely unphysical and leads to divergence.

Thank you for the answer!

[vinerm]

141 Pa is free stream pressure, however, it appears that you are using that value as Initial Supersonic pressure as well, leading to low pressure at the back of the body. Static pressure should settle down to 141 Pa but for initialization, you have to use higher value. Instead of mesh, could you attach your CAD model here? CAD file would be much smaller.

[Captain Convergence]

I have attached a .zip with the geometry in .igs format in case you don´t have ANSYS 19 (i couldn´t upload it in .igs format directly).

By now I am trying with pressure far-field where I only specify the Mach number (9.6), static pressure (141 Pa) and static temperature (47 K). But you are right I will have to set a Initial Supersonic pressure once I switch to real-gas model because I won´t be able to use pressure far-field. In another thread you commented that it should be close to the specified total pressure at the inlet, I will try to do so once I am at that stage

[vinerm]

I have multiple versions of Ansys, starting from v11 all the way upto 2020 R1. So, it would be better if you share SCDM or DM file, provided you used those tools. IGES may have data loss.

[Captain Convergence]

Done, I have uploaded the updated .zip with the DM file

[vinerm]

It is a delta wing and you are using 2D model. As far as simulation is concerned it should work but the results will be different from the paper. Are you using 2D planar simulation?

[Captain Convergence]

I am aware of that, I started doing a 2D case to test how the solver controls and my real-gas model work. If I haved had started with the 3D case, it would take me ages to test my solver settings.

However it is not working for me in 2D even though I am using a conservative solver configuration (i.e. explicit mode and low courant number).

[vinerm]

Even in 2D, you appear to be using a very fine mesh. Benefit of running in 2D is being offset due to that, I suppose. Anyway, I tried with Inviscid model and fmg initialization using far-field boundary. I did not use symmetry. Case runs alright with first-order, Implicit. Did not try explicit yet. And I suppose you are modeling viscous flow, are you? Which turbulence model are you using then?

[Captain Convergence]

So have you mirror the domain? I don't think I can use pressure far-field where I have my symmetry because it is in contact with the body.

Really? Did it work for you? With the same flow conditions I specified in the first post? I haven´t tried first order momentum equation, only second order. Would you mind attaching an image with the Mach number contour right after the fmg-initialization?

I was planning to do an study with inviscid, k-epsilon and SST and compare them with the experimental data.

[vinerm]

Pressure, Mach number, Velocity, and Density values right after fmg-initialization are attached. Far-field pressure is 141 Pa abs. and Temperature is 47 K

[vinerm]

These are the images after 500 iterations with Implicit Roe-FDS with Pseudo-Transient.

[Captain Convergence]

Thank you very much for the contours!

I guess that you have used fmg-initialization with the default values right?

Then the issue in my case is the symmetry? I don't really understand how it affects the pressure far-field. If it its, it means that I won't be able to use symmetry in my 3D case and my computational cost will increase dramatically.

[vinerm]

Pressure far-field condition cannot touch any other boundary. So, you have to use full body. But you may not require the resolution you are using.

[vinerm]

There are two very important differences in yours and my cases. First one is the placement of the upstream boundary. Though I have also kept it close to the wing, but it is still farther than in your case. It needs to be even farther upstream. Secondly, the shape of the domain. It is recommended to use a parabolic shape instead of a rectangular or some other shape. You might be able to work with symmetry but you have to change the shape of the outer domain to a parabolic one and move the inlet upstream. That should make far-field work properly.

[Captain Convergence]

I tried to do the same changes (see the attached image) but I still having the same issue, the fmg doesn't even converge. I have attached also an extract of the journal file that I am using, please run it in your Fluent and let me know if you have any issue. I am very confused with my method.

Thank you for your time, I really appreciate it!

[vinerm]

Default initialization in Fluent is Hybrid. You have to set it to Standard, then use compute from far-field, and then initialize. After that, initialize with fmg. Set operating pressure to exactly 0.

[Captain Convergence]

Thank you so much for the tip, that fixed the issue with the initialization, is someone is reading this thread, the way to do it from command line is:

;;--------------------------------------------------------------------------------------------------
;; INITIALIZATION
(ti-menu-load-string (format #f "/solve/initialize/compute-defaults pressure-far-field inlet \n"))
(ti-menu-load-string (format #f "/solve/initialize/initialize-flow yes \n"))
(ti-menu-load-string (format #f "/solve/initialize/fmg-initialization yes \n"))
;;--------------------------------------------------------------------------------------------------

However I am not sure if you have pushed enough the simulation but due to the local velocity peaks from the initialization (see the attached image), the simulation starts to diverge because it doesn't handle properly the shockwave formation. I am starting to think that I should switch to an structured mesh with quads because the triangles might be inducing an intense false diffusion.

[vinerm]

Yes, structured mesh is better. That will reduce the mesh count. I didn't use structured mesh but quadrilaterals. With that, I was able to run even with second order.