[mkraposhin]

Hi, Chirag

I finieshed calculations with your example, you can see results in attached files - Mach number, temperature and velocity magnitude distributions.

As you can see, Ma number (at least at spike) have a very good match with Fluent, however, temperature and velocity fields are over predicted. This can be due to wrong inlet B.C. I think, it's time to ask authors of original research

[chirag]

Hello Sir,
I tried to simulate the new geometry ( with slight diverging section) in fluent and OF with varying viscosity but constant specific heat. The inlet pressure is ramped from 100 to 20000 Pa (as per your table). I have to do the post processing of fluent and then make one to one comparison.
The maximum velocity in both the cases is observed to be exactly matching (around 3300 m/s). I modified the minimum pressure from 2 Pa to 1e-8 after 20000 iterations. Its interesting to know that the limitation applied is not needed after stabalization of flow near the inlet region. The pressure in OF dips to minimum value of 0.3 Pa.
I have completed around 27000 iterations in PisoCentralFoam and the flow in the domain has not yet stabalized (may be another 10000 iterations will do!). Attached are plot of T and U comparison with experimental data. I will update the fluent results soon in this plot with diverging inlet geometry.
(unfortunately my server has some problems so m doing it on my laptop and its really taking alot of time . Once I have my server working, I can download the fluent case files and then make a comparison)

The case got blowed up due to negative epsilon and k at something around 25000 iterations. So, I modified the rdeltaTcoeff to lower value of 0.005 (it diverged at 0.01). and deltaTdampeningcoeff to 0.9.

[mkraposhin]

Yes, you must do more iterations.
Also, to limite pressure and/or temperature or density, you must use fvOptions
To use them, update your pisoCentralFoam and compressibleTools from github.

Also, i want to make this case as a tutorial for my solver. Do you permit to use your blockMeshDict file? If yes, i will upload it to github tomorrow.

[chirag]

You surely can use it. I will share with you the final results of the fluent which will also help in validating it if needed.
I had few doubts:
1) I just wanted to know more about the localEuler. Is there some publication over this method? I tried to search but couldn't find any. There are few posts but not very clear.
2) Why $scalarAdvScheme is generally used if we have advanced schemes like vanleer, MUSCL? You have already said that other schemes will work perfectly!
I actually didn't understand the way $scalarAdvScheme it works and wanted to know more about it.
3) Why isn't pisoCentralFoam, compressible library, etc. part of openfoam installation?
Regards,

[chirag]

Originally Posted by mkraposhin

Hi, Chirag

I finieshed calculations with your example, you can see results in attached files - Mach number, temperature and velocity magnitude distributions.

As you can see, Ma number (at least at spike) have a very good match with Fluent, however, temperature and velocity fields are over predicted. This can be due to wrong inlet B.C. I think, it's time to ask authors of original research

Hello Sir,
Do we need to compulsorily use the heatflux B.C on the nozzle wall? It causes problems in convergence and over prediction of temperature slightly in flow field (observed in fluent).
Thanks,

[mkraposhin]

Originally Posted by chirag

1) I just wanted to know more about the localEuler. Is there some publication over this method? I tried to search but couldn't find any. There are few posts but not very clear.

It's a method when ddt scheme is local for all cells, depending on local Courant number. During iteration process, this fictitious time derivatives are vanishes and solution tends to steady-state

Originally Posted by chirag

2) Why $scalarAdvScheme is generally used if we have advanced schemes like vanleer, MUSCL? You have already said that other schemes will work perfectly!
I actually didn't understand the way $scalarAdvScheme it works and wanted to know more about it.

$scalarAdvScheme - is the name of variable, that stores type of scheme - "string".
you can set it to vanLeer with string

    scalarAdvScheme vanLeer;

then you can use it anywhere

    div(phiPos,h) Gauss $scalarAdvScheme; //Equal to Gauss vanLeer in this case

You must know, that for hybrid scheme, all convection terms and interpolated values, marked with "reconstruct" should be discretized with the same scheme

Originally Posted by chirag

3) Why isn't pisoCentralFoam, compressible library, etc. part of openfoam installation

This is my goal. But i have to be sure, that pisoCentralFoam is really usefull

[mkraposhin]

Originally Posted by chirag

You surely can use it. I will share with you the final results of the fluent which will also help in validating it if needed.

I will upload my case setup to github tomorrow

[mkraposhin]

Originally Posted by chirag

Hello Sir,
Do we need to compulsorily use the heatflux B.C on the nozzle wall? It causes problems in convergence and over prediction of temperature slightly in flow field (observed in fluent).
Thanks,

My opininon - we must try to setup our case as more close as it possible to fluent case. Then, after that we can try to setup it with more physically assumptions (if we decide, that assumptions in previous study were not correct)

[mkraposhin]

Hi,

I uploaded my version of case for 100Pa to git hub. It is here https://github.com/unicfdlab/realLif...lasmaExpansion

[Proportion]

Originally Posted by mkraposhin

Hi,
You must compile library with script ./makeLib.sh

Hi,

I' working on a case similar to the one dicussed here and I'm trying to use your libcompressibletools to get it to converge. Unfortunately I encountered the same error reported by chirag in #14. I compiled it with ./makeLib.sh.

Can somebody please help me with the installation process? I attached the log file.
Thanks in advance!