|
[Sponsors] |
Diverging solution from Pressure-based to Density-based |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
April 20, 2020, 06:44 |
Diverging solution from Pressure-based to Density-based
|
#1 |
New Member
Killian
Join Date: Nov 2017
Posts: 26
Rep Power: 8 |
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 |
|
April 20, 2020, 06:58 |
Objective
|
#2 |
Senior Member
|
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?
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. |
|
April 20, 2020, 06:59 |
|
#3 | |
New Member
Killian
Join Date: Nov 2017
Posts: 26
Rep Power: 8 |
Quote:
https://tfaws.nasa.gov/TFAWS11/Proce...aXHURRLa3gRX1E |
||
April 20, 2020, 07:13 |
Numerics
|
#4 |
Senior Member
|
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.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority. |
|
April 20, 2020, 08:01 |
|
#5 | |
New Member
Killian
Join Date: Nov 2017
Posts: 26
Rep Power: 8 |
Quote:
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. |
||
April 20, 2020, 09:44 |
|
#6 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,676
Rep Power: 66 |
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. |
|
April 20, 2020, 11:27 |
|
#7 | |
New Member
Killian
Join Date: Nov 2017
Posts: 26
Rep Power: 8 |
Quote:
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. |
||
April 20, 2020, 11:44 |
|
#8 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,676
Rep Power: 66 |
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. |
|
April 20, 2020, 19:53 |
|
#9 | |
New Member
Killian
Join Date: Nov 2017
Posts: 26
Rep Power: 8 |
Quote:
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) : 93803212_1506443509525076_2617933053976117248_n.png 94569242_250987429370051_8343956278745235456_n.png But do you know why I have this kind of curves compared to their ones? Is it related to my mesh? 94123569_637110510176368_3397079605104869376_n.jpg As you can see, the the curves are steeper. |
||
April 21, 2020, 03:35 |
|
#10 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,676
Rep Power: 66 |
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. |
|
April 21, 2020, 07:44 |
|
#11 | |
New Member
Killian
Join Date: Nov 2017
Posts: 26
Rep Power: 8 |
Quote:
|
||
April 21, 2020, 14:57 |
|
#12 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,676
Rep Power: 66 |
I have no comments on the mesh because I have no idea what it looks like.
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Pressure fields in FOAM, p field, total pressure, etc. | Tobi | OpenFOAM Post-Processing | 9 | March 25, 2022 01:33 |
Compressible Flow on Pressure Based | Daryun | FLUENT | 2 | July 5, 2019 10:44 |
Pressure and density based solver | JOKER | FLUENT | 0 | February 18, 2011 09:58 |
Pressure gradient in UDF for density based solver | matzb | FLUENT | 0 | February 22, 2010 06:34 |
Hydrostatic pressure in 2-phase flow modeling (long) | DS & HB | Main CFD Forum | 0 | January 8, 2000 15:00 |