CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Verification & Validation

Unexpected jump in Velocity & Temp across shock using pisoCentralFoam &rhoCentralFoam

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree4Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 2, 2016, 06:01
Default
  #21
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21
mkraposhin is on a distinguished road
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
Attached Images
File Type: jpg Ma-steady-state.jpg (31.6 KB, 51 views)
File Type: jpg T-steady-state.jpg (27.1 KB, 41 views)
File Type: jpg U-steady-state.jpg (29.3 KB, 35 views)
chirag likes this.
mkraposhin is offline   Reply With Quote

Old   February 2, 2016, 08:43
Default promising results from pisoCentralFoam
  #22
New Member
 
chirag khalde
Join Date: Sep 2011
Posts: 22
Rep Power: 15
chirag is on a distinguished road
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.
Attached Images
File Type: png Untitled_Umag.png (39.9 KB, 43 views)
File Type: png Untitled_T.png (40.4 KB, 33 views)

Last edited by chirag; February 2, 2016 at 08:56. Reason: forgot to put the title
chirag is offline   Reply With Quote

Old   February 2, 2016, 11:40
Default
  #23
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21
mkraposhin is on a distinguished road
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 likes this.
mkraposhin is offline   Reply With Quote

Old   February 2, 2016, 12:00
Default
  #24
New Member
 
chirag khalde
Join Date: Sep 2011
Posts: 22
Rep Power: 15
chirag is on a distinguished road
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
chirag is offline   Reply With Quote

Old   February 2, 2016, 12:23
Default
  #25
New Member
 
chirag khalde
Join Date: Sep 2011
Posts: 22
Rep Power: 15
chirag is on a distinguished road
Quote:
Originally Posted by mkraposhin View Post
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,
chirag is offline   Reply With Quote

Old   February 2, 2016, 13:44
Default
  #26
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21
mkraposhin is on a distinguished road
Quote:
Originally Posted by chirag View Post
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

Quote:
Originally Posted by chirag View Post
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
Code:
    scalarAdvScheme vanLeer;
then you can use it anywhere
Code:
    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

Quote:
Originally Posted by chirag View Post
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 is offline   Reply With Quote

Old   February 2, 2016, 13:46
Default
  #27
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21
mkraposhin is on a distinguished road
Quote:
Originally Posted by chirag View Post
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 is offline   Reply With Quote

Old   February 2, 2016, 13:48
Default
  #28
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21
mkraposhin is on a distinguished road
Quote:
Originally Posted by chirag View Post
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 is offline   Reply With Quote

Old   February 3, 2016, 04:20
Default
  #29
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 355
Rep Power: 21
mkraposhin is on a distinguished road
Hi,

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

Old   July 14, 2017, 09:10
Default Trouble installing libcompressibletools
  #30
New Member
 
P. H.
Join Date: Jul 2017
Posts: 5
Rep Power: 9
Proportion is on a distinguished road
Quote:
Originally Posted by mkraposhin View Post
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!
Attached Files
File Type: txt log_makeLib.txt (6.5 KB, 3 views)
Proportion is offline   Reply With Quote

Reply

Tags
pisocentralfoam, rhocentralfoam, shock wave, validation

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 09:05.