|
[Sponsors] |
Unexpected jump in Velocity & Temp across shock using pisoCentralFoam &rhoCentralFoam |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
February 2, 2016, 06:01 |
|
#21 |
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21 |
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
__________________
MDPI Fluids (Q2) special issue for OSS software: https://www.mdpi.com/journal/fluids/..._modelling_OSS GitHub: https://github.com/unicfdlab Linkedin: https://linkedin.com/in/matvey-kraposhin-413869163 RG: https://www.researchgate.net/profile/Matvey_Kraposhin |
|
February 2, 2016, 08:43 |
promising results from pisoCentralFoam
|
#22 |
New Member
chirag khalde
Join Date: Sep 2011
Posts: 22
Rep Power: 15 |
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. Last edited by chirag; February 2, 2016 at 08:56. Reason: forgot to put the title |
|
February 2, 2016, 11:40 |
|
#23 |
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21 |
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.
__________________
MDPI Fluids (Q2) special issue for OSS software: https://www.mdpi.com/journal/fluids/..._modelling_OSS GitHub: https://github.com/unicfdlab Linkedin: https://linkedin.com/in/matvey-kraposhin-413869163 RG: https://www.researchgate.net/profile/Matvey_Kraposhin |
|
February 2, 2016, 12:00 |
|
#24 |
New Member
chirag khalde
Join Date: Sep 2011
Posts: 22
Rep Power: 15 |
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, Last edited by chirag; February 2, 2016 at 12:20. Reason: wrong formulation of question |
|
February 2, 2016, 12:23 |
|
#25 | |
New Member
chirag khalde
Join Date: Sep 2011
Posts: 22
Rep Power: 15 |
Quote:
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, |
||
February 2, 2016, 13:44 |
|
#26 | ||
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21 |
Quote:
Quote:
you can set it to vanLeer with string Code:
scalarAdvScheme vanLeer; Code:
div(phiPos,h) Gauss $scalarAdvScheme; //Equal to Gauss vanLeer in this case This is my goal. But i have to be sure, that pisoCentralFoam is really usefull
__________________
MDPI Fluids (Q2) special issue for OSS software: https://www.mdpi.com/journal/fluids/..._modelling_OSS GitHub: https://github.com/unicfdlab Linkedin: https://linkedin.com/in/matvey-kraposhin-413869163 RG: https://www.researchgate.net/profile/Matvey_Kraposhin |
|||
February 2, 2016, 13:46 |
|
#27 | |
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21 |
Quote:
I will upload my case setup to github tomorrow
__________________
MDPI Fluids (Q2) special issue for OSS software: https://www.mdpi.com/journal/fluids/..._modelling_OSS GitHub: https://github.com/unicfdlab Linkedin: https://linkedin.com/in/matvey-kraposhin-413869163 RG: https://www.researchgate.net/profile/Matvey_Kraposhin |
||
February 2, 2016, 13:48 |
|
#28 |
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21 |
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)
__________________
MDPI Fluids (Q2) special issue for OSS software: https://www.mdpi.com/journal/fluids/..._modelling_OSS GitHub: https://github.com/unicfdlab Linkedin: https://linkedin.com/in/matvey-kraposhin-413869163 RG: https://www.researchgate.net/profile/Matvey_Kraposhin |
|
February 3, 2016, 04:20 |
|
#29 |
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21 |
Hi,
I uploaded my version of case for 100Pa to git hub. It is here https://github.com/unicfdlab/realLif...lasmaExpansion
__________________
MDPI Fluids (Q2) special issue for OSS software: https://www.mdpi.com/journal/fluids/..._modelling_OSS GitHub: https://github.com/unicfdlab Linkedin: https://linkedin.com/in/matvey-kraposhin-413869163 RG: https://www.researchgate.net/profile/Matvey_Kraposhin |
|
July 14, 2017, 09:10 |
Trouble installing libcompressibletools
|
#30 |
New Member
P. H.
Join Date: Jul 2017
Posts: 5
Rep Power: 9 |
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! |
|
Tags |
pisocentralfoam, rhocentralfoam, shock wave, validation |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
wrong velocity & temp at initialization | Leo | FLUENT | 1 | October 15, 2007 10:42 |
Pressure jump on supersonic velocity inlet | Viktor | FLUENT | 0 | August 9, 2007 00:23 |
Variables Definition in CFX Solver 5.6 | R P | CFX | 2 | October 26, 2004 02:13 |
Porous jump and velocity | Christian | FLUENT | 6 | May 21, 2003 13:24 |
Terrible Mistake In Fluid Dynamics History | Abhi | Main CFD Forum | 12 | July 8, 2002 09:11 |