Diverging solution from Pressure-based to Density-based
 

Hello everyone,

I try to simulate a convergent-divergent nozzle flow based on this subject https://ntrs.nasa.gov/search.jsp?R=19820006179
Following the method used by these people: https://tfaws.nasa.gov/TFAWS11/Proce...aXHURRLa3gRX1E

The methods used are:

- Pressure Based Coupled Solver (PBCS) with 1/ 2nd order for all equations OR 2/ PRESTO for Pressure and QUICK for other equations

- Density Based Solver (DBNS) with 2nd order for all equations

Input parameters:

Material: Air (ideal-gas)

Model: SST k-omega (2 equ.)

Boundary conditions: 1 pressure inlet (2.5 atm), 1 pressure outlet (1 atm)

Solution method: ROE-FDS - Least square - 2nd order

Initialization method: Hybrid or Standard

I successfully represented the model with the Pressure-based solver both for 2nd order and PRESTO/QUICK (as you can see on images attached).

But as soon as I move to the Density based solver, I get a diverging solution, even if I change the Hybrid initialization to the Standard initialization. It always starts pretty well but diverges after around 250 iterations, when the mach disk appears. You can see it on the other pictures attached (I stopped the simulation right before the divergence).

I tried to change settings such as turbulent model (going from k-omega to k-epsilon etc.) and also inlet pressure, pseudo transient on/off... but it always diverges. I have the same problem on other projects but here, I don't understand why I have good results with Pressure based solver and not with Density based solver.

At first, I thought it was related to Mesh quality but I tried on an other project (with good results on density based solver) to move from a good mesh (with a converged solution) to coarse mesh, and the solution still converges. I think the problem is related to the shocks, but I can't verify it.

Have you any thoughts about from where does the problem comes from?

Best regards,

Killian

Objective
 

If you are getting good results with PBNS, why do you want to use DBNS? Are you interested in comparing the results for both solvers?

Sure! I would like to compare both solvers, as done in the paper linked above.

https://tfaws.nasa.gov/TFAWS11/Proce...aXHURRLa3gRX1E

Numerics
 

Assuming the physical setup is as per the document you are referring, did you try AUSM+ instead of Roe FDS. Since you mentioned the problem appears as soon as Mach disk appears, AUSM+ might be able to handle that better.

I also tried AUSM+, as it's well suited for shocks. But the problem is still the same..

Yesterday, I tried to move from Implicit formulation to Explicit formulation and the solution is converging pretty well (residuals are quite stable) but it took approximately 6500 iterations to get the same result than a classical 300 iterations Implicit formulation, so I'm not really satisfied with this.

You can probably get it to work eventually if you just play with the solver settings.


6500 iterations is not a lot and I would never trust results with only 300 iterations in them.

I tried to play with the solver settings (select/unselect pseudo-transient, changing boundary conditions etc.) but nothing worked.

My sentence was more like "To get to the point where I am after 300 iterations with PBCS, I need to do 6500 iterations with DBNS and I need to use Explicit formulation". I don't assume that the 300 iterations made with PBCS are enough, but simply that it's a quite stabilized solution :) You can clearly see it with the pictures attached.

I have no problem with the use of Explicit formulation, but I don't understand why the solution doesn't work with Implicit formulation, as soon as the shock is appearing.

By playing, I don't mean changing schemes. Keep all models the same and play with only the initialization & the solution controls. E.g. with a low enough Courant number, it should converge, maybe in 10,000 iterations.


There are a ton of accelerators under the hood used to speed up convergence (so that it doesn't take 6000 iterations) and the cost of accelerating the solution is that it become less stable. This stuff happens all the time. The DBNS is a coupled solver which is naturally faster (and less stable) than PBNS.

Ok so I know what the problem was: Fluent automatically changed the CFL number to 5 when I switched from PBCS to DBNS, and I didn't noticed that since it was initially set to 1. Now I understand why I got this fast divergence..


Here's what I get with a CFL = 1, DBNS, AUSM and 10 000 iterations (far better) :


Attachment 76756 Attachment 76757

But do you know why I have this kind of curves compared to their ones? Is it related to my mesh?

Attachment 76758

As you can see, the the curves are steeper.

That's par for the course. Numerically trying to resolve discontinuities and get really nice steep-fronted solutions is tough without specialized schemes. Probably you are predicting the location of the shocks pretty well (but not their thickness).

Actually if you compare your numerical results to their numerical results on slide 18, they're very similar.

Sure, I understand. Do you think the better curvature they get is related to the mesh quality (slide 18)? They better represent the experimental data, with the same boundary conditions and methods so I guess this is related to the mesh.

I have no comments on the mesh because I have no idea what it looks like.

Here's my mesh near the wall (I know it's not a very fine mesh):


Attachment 76799