
[Sponsors] 
December 23, 2019, 06:10 

#21 
Senior Member
Join Date: Dec 2019
Posts: 215
Rep Power: 7 
Hi all,
@tas38: Yes this unphysical phenomenon exist also for a fixed velocity at the inlet. I also tried changing the schemes and so on, but nothing helped. @tobi: I have had the best results with rhoCentralFoam, thats why I am using it. Tbh I have not used rhoPimpleFoam yet, but I think I should try it soon. It might be easier to work with this solver since you can work with relaxations, what cant be done with rhoCentralFoam Good luck on your case! I have finally solved the problem. For anyone with the same issue: I have filled the injector with the static pressure and static temperature that equals the total pressure and total temperature at the inlet. Since the velocity is 0 at t = 0, they equal the total pressure/temperature. I had no more issues with convergence and everything works stable. The strange phenomenon did not appear anymore. I would like to thank everyone for the kind help and wish you all merry Christmas and a good start in the new year! 

December 23, 2019, 16:28 

#22 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 52 
Hi,
the only thing I can tell you about the rhoPimpleFoam solver is the fact about relaxation. Generally, we only relax the field for the pressure. However, for transonic behavior it is common to make at least the pressure equation diagonal dominant. We can achieve that using the equation relaxation factor for p and set it equal to 1. If we check out some transonic tutorials, we can see that this is set. In addition, we could use the PIMPLE algorithm to get a more accurate and stable result (not running in PISO mode). Especially for more stiff problems this is recommended. I would say it is worth to check but, as I already said, I am not familiar with transonic and supersonic calculations.
__________________
Keep foaming, Tobias Holzmann 

December 29, 2019, 11:17 

#23 
Senior Member
Join Date: Dec 2019
Posts: 215
Rep Power: 7 
Thanks for the informations!
I think I will give it a try and see whether it solve behaves more stable. You can use the pimple algorithm with sonicFoam too, but the solver gives worse result compared to rhoCentralFoam. Since rhoPimpleFoam is also density based I think it is definitly worth a try! 

December 29, 2019, 16:41 

#24 
Member
giovanni
Join Date: Sep 2017
Posts: 50
Rep Power: 9 
hi guys, regarding this case, I would ask you in the case of a variable total pressure at the inlet how is possible to specify a variable total temperature as said before? thanks


December 30, 2019, 07:24 

#25 
Senior Member
Join Date: Dec 2019
Posts: 215
Rep Power: 7 
There is no standard way to do it. I guess you have to make your own BC.
Last edited by shock77; December 30, 2019 at 09:37. 

March 19, 2020, 13:25 

#26 
Member
Giovanni Caramia
Join Date: Mar 2009
Location: Bari, ITALY
Posts: 58
Rep Power: 17 
Here there is the link for version 1.7.x source file. It would be nice to know why this bc is no longer present in the successive releases
https://github.com/OpenCFD/OpenFOAM...dTotalPressure Hope this could help. 

June 2, 2021, 16:37 

#27  
New Member
Lewis
Join Date: Jun 2021
Posts: 26
Rep Power: 5 
Quote:
Hi Tobi, can you elaborate on this a little? Why would the flow keep accelerating? I'm trying to do something similar here but my setup fails after a while: Correct BCs for known outlet conditions and unknown inlet conditions 

November 17, 2021, 12:25 

#28  
Member
Utkun Malkocoglu
Join Date: Feb 2017
Posts: 36
Rep Power: 9 
Quote:
I am also studying the same type of configuration, an injector is located at the bottom of domain and sonic jet leaves the injector through supersonic crossflow. I tried numerous boundary conditions, schemes etc. However, I could not get the results that expected. If I give pressure ratio (PR, jet total pressure divided by crossflow static pressure) more than 510, rhoCentralFoam crashes. My configuration contains PR~150 and solver can not continue to solve with this PR. A shock like zone occurs just after the injector inlet and never disappear until the solver blows. I also tried the thing @shock77 said in the quotation, but it did not work, too. I am struggling with it for months and I can not do anything extra because I feel I ran out of the options I can do. So if anyone could help me, I would be super thankful to him/her. Thanks in advance, stay safe and healthy, Malkocoglu 

November 17, 2021, 16:30 

#29 
Senior Member
Join Date: Dec 2019
Posts: 215
Rep Power: 7 
Could you share your BCs, schemes and your Conumber? Also an image would be helpful, if you can share it.


November 18, 2021, 04:46 

#30  
Member
Utkun Malkocoglu
Join Date: Feb 2017
Posts: 36
Rep Power: 9 
Quote:
Firstly, thank you for your attention and quick response. To clarify, I have to say that I am currently using k  omega SST turbulence model with symmetry (I am trying to solve half of the domain). I hope that I can write in clear way, if this is not the case please warn me on necessary points. I will list them in order: Boundary Conditions I wrote the commented BCs which means I also tried them.
system/fvSchemes Code:
/** C++ **\ =========  \\ / F ield  OpenFOAM: The Open Source CFD Toolbox \\ / O peration  Website: https://openfoam.org \\ / A nd  Version: dev \\/ M anipulation  \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // fluxScheme Kurganov; ddtSchemes { default Euler; //Euler; //CrankNicolson 0.5; } gradSchemes { default cellMDLimited Gauss linear 1.0; //cellMDLimited Gauss linear 1.0; grad(U) cellMDLimited Gauss linear 1.0; //cellLimited<cubic> 1.5 Gauss linear 1.0; grad(e) cellMDLimited Gauss linear 1.0; //cellLimited<cubic> 1.5 Gauss linear 1.0; // grad(R) cellMDLimited Gauss linear 1.0; //cellMDLimited Gauss linear 1.0; grad(k) cellMDLimited Gauss linear 1.0; //cellLimited<cubic> 1.5 Gauss linear 1.0; grad(omega) cellMDLimited Gauss linear 1.0; //cellLimited<cubic> 1.5 Gauss linear 1.0; // grad(p) Gauss linear 0.33333; } divSchemes { default none; div(phi,U) bounded Gauss vanLeerV outletStabilisedV grad(U); //bounded Gauss linearUpwindV grad(U); div(phi,e) bounded Gauss vanLeer outletStabilised grad(e); //bounded Gauss linearUpwind grad(e); div(phi,k) bounded Gauss vanLeer outletStabilised grad(k); //bounded Gauss linearUpwind grad(k); div(phi,omega) bounded Gauss vanLeer outletStabilised grad(omega); //bounded Gauss linearUpwind grad(epsilon); div(((rho*nuEff)*dev2(T(grad(U))))) bounded Gauss vanLeer; //linearUpwind; //bounded Gauss linearUpwind; div(tauMC) Gauss linear; } laplacianSchemes { default Gauss linear limited 1.0; } interpolationSchemes { default linear; reconstruct(rho) vanLeer; reconstruct(T) vanLeer; reconstruct(p) vanLeer; reconstruct(k) vanLeer; reconstruct(omega) vanLeer; reconstruct(e) vanLeer; reconstruct(U) vanLeerV; snGradSchemes { default limited 1.0; //limited 0.5; //limited corrected 0.5; } wallDist { method meshWave; } // ************************************************************************* // I defined my Co as min ~0.1 and max ~0.5. Nowadays, it is around ~0.2. The domain I have included several figures to elucidate the situation, please see the attachment. These figures point to the situation where the PR= 5 as I said above. So, I have the problem on maintaining PR ~ 150 in whole injector and just around the injector opening section. By looking the graph among this figures, the ratio is approximately maintained just after the injector inlet but it has to be at the location which injector meets the crossflow domain. In my opinion, due to this mismatch there are not any jet  crossflow related interaction phenomena over the domain (at least, in the way that it is expected). Thank you one more time for your interest, hopefully this information is adequate as much as it can be. If you wonder something different than the given, I can also provide them. Finally, I would be appreciated so much if we can respond to each other at least once in a day (if it suits to your daily programme), because I have very limited time after hopeless trials. Thanks, stay safe and healthy, Malkocoglu 

November 18, 2021, 05:38 

#31 
Senior Member
Join Date: Dec 2019
Posts: 215
Rep Power: 7 
Hi,
I have never used those "freeStream" boundary conditions, so I cant tell anything about them. But it seems your inlet boundary conditions are cosing the problems. Also I think those "bounded" schemes are for stationary flows, you should also look into that. I would try the following at the inlet: Either totalPressure + pressureInletOutletVelocity or fixedValue for p and for U 

November 18, 2021, 05:55 

#32  
Member
Utkun Malkocoglu
Join Date: Feb 2017
Posts: 36
Rep Power: 9 
Quote:
Quote:
Quote:
Quote:
Hopefully, I will try and write back here at 1011 pm GMT +3. Best, Malkocoglu 

November 18, 2021, 07:28 

#33 
Senior Member
Join Date: Dec 2019
Posts: 215
Rep Power: 7 
In terms of stability, I had the best results with totalPressure, totalTemperature and pressureInletOutletVelocity. But I guess every case is somehow different in the end.
Depending on wether you are interested in dynamic behaviour or not: You could use uniformTotalPressure to define a total pressure rise over time. With that, you can slowly ramp up your pressure, which is far easier to handle for a solver than a step input. On the keyword "bounded" I think you should read this: https://openfoam.org/release/220/n...sboundedness/ 

November 18, 2021, 08:27 

#34  
Member
Utkun Malkocoglu
Join Date: Feb 2017
Posts: 36
Rep Power: 9 
Quote:
Quote:
Quote:
"Compressible solvers for transient problems generally use the PIMPLE algorithm, which supports partial convergence of intermediate iterations. The solution may benefit from the use of the bounded form of convection but, in such cases, the corresponding bounded time derivative must also be included, ..." Even if I use a solver belonging to PIMPLE, it stands right for my case. So, I understand that if I'm going use bounded for convective term, I also have to use for time derivative. I did not know that, thank you. 

November 18, 2021, 08:33 

#35 
Senior Member
Join Date: Dec 2019
Posts: 215
Rep Power: 7 
I have tried different ratios like 10/1, 50/1, 100/1 and 200/1 as far as I remember. It worked with the solution I have suggested.
In your case there is some kind of pushbackeffect into your inlet. I am not sure why it is caused, but I can only imagine that the totalPressure at your inlet is smaller than outside for some reason. 

November 18, 2021, 08:48 

#36  
Member
Utkun Malkocoglu
Join Date: Feb 2017
Posts: 36
Rep Power: 9 
Quote:
Quote:
Anyway, I will try with your suggestions and in the case I can not write today please do not disappear on the forum , I need to talk about somebody like you who had an experience on this particular problem. How many times I said I do not know but thank you one more time. 

November 18, 2021, 08:55 

#37 
Senior Member
Join Date: Dec 2019
Posts: 215
Rep Power: 7 
No, it was some kind of orifice.
I feel you, no worries. I have seen those injector cases a few times, maybe you can try to find their BCs and use those? If I had to setup that case, I would try the following first: Inlet: totalPressure, totalTemperature, pressureInletOutletVelocity crossflowInlet: fixedValue for p, T and U outlets with shockwaves: waveTransmissive for p, U and zeroGradient for T outlet with no shockwaves involed: inletOutlet On the schemes: I think there is rather a problem with the BCs than the schemes, because of the weird phenomena at the inlet. We should focus on those. 

November 18, 2021, 09:13 

#38  
Member
Utkun Malkocoglu
Join Date: Feb 2017
Posts: 36
Rep Power: 9 
You can not guess how grateful I am.
Quote:
Quote:
Quote:


November 19, 2021, 05:27 

#39 
Senior Member
Join Date: Dec 2019
Posts: 215
Rep Power: 7 
Isnt your injector basically a jet inlet?
I dont think there should be any troubles. I think in that case it behave like a zeroGradient BC. But I am not 100% sure. It doesnst look like a mesh problem to me. 

November 19, 2021, 06:14 

#40  
Member
Utkun Malkocoglu
Join Date: Feb 2017
Posts: 36
Rep Power: 9 
Quote:
Best, Malkocoglu 

Tags 
rhocentralfoam, totalpressure 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
totalPressure (why flux direction dependend)  Tobi  OpenFOAM Running, Solving & CFD  3  October 17, 2019 23:27 
Need info about totalPressure boundary condition  sahmed  OpenFOAM Running, Solving & CFD  4  December 4, 2018 22:23 
About the totalPressure BC  fmerk  OpenFOAM Running, Solving & CFD  1  September 25, 2017 18:53 
totalPressure boundary :Performance Curve (constant RPM)  nash  OpenFOAM Running, Solving & CFD  0  September 6, 2013 12:34 
Totalpressure Ansys  Leuchte  CFX  2  April 9, 2013 19:56 