CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM News & Announcements > OpenFOAM Announcements from Other Sources

QGDsolver - OpenFOAM computational framework for fluid flows based on regularized equ

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

Like Tree11Likes
  • 8 Post By mkraposhin
  • 1 Post By mkraposhin
  • 1 Post By mkraposhin
  • 1 Post By mkraposhin

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 25, 2020, 11:41
Default QGDsolver - OpenFOAM computational framework for fluid flows based on regularized equ
  #1
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 343
Rep Power: 18
mkraposhin is on a distinguished road
QGDsolver is OpenFOAM framework for simulation of fluid flows using regularized equations approach. It contains library for approximation of partial derivatives at face centers of unstructured grids and a set of OpenFOAM solvers:
  • QGDFoam - solver for compressible viscous perfect gas flows in a wide Mach number range - from 0 to infinity
  • QHDFoam - solver for incompressible viscous fluid flows with buoyancy force
  • particlesQGDFOam - solver for compressible viscous perfect gas flows in a wide Mach number range with particles - from 0 to infinity
  • particlesQHDFoam - solver for incompressible viscous fluid flows with buoyancy force with particles
  • SRFQHDFoam - solver for incompressible viscous fluid flows in rotating frame of reference with buoyancy force
  • QHDDyMFoam - solver for incompressible viscous fluid flows in domains with deforming boundary and with buoyancy force
  • interQHDFoam - solver for incompressible 2-phase viscous fluid flows with buoyancy force and surface tension
  • reactingLagrangianQGDFoam - solver for reacting multicomponent compressible viscous perfect gas flows in a wide Mach number range with particles - from 0 to infinity
  • scalarTransportQHDFoam - solver for scalar transport equation to demonstrate the very basics of QGD/QHD equations principles

Generally speaking, QGD/QHD framework offers an alternative to PISO/SIMPLE and Riemann-solvers approach to simulate various flow phenomena on unstructured grids. And sometimes it could be superior comparing to mentioned techniques.

The framework could be downloaded HERE: https://github.com/unicfdlab/QGDsolver

The presentation covering some theory and basics of the implemeted approach could be downloaded HERE: https://github.com/unicfdlab/QGDsolver/blob/master/qgd-framework-2020-final.pdf

Please, do not hesitate to ask for assistance on how to setup the case or on how to derive new equations for your problem using regularized hydrodynamic approach
JBeilke, olesen, dybuk and 5 others like this.

Last edited by mkraposhin; May 26, 2020 at 03:15.
mkraposhin is offline   Reply With Quote

Old   October 2, 2020, 07:43
Default
  #2
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 343
Rep Power: 18
mkraposhin is on a distinguished road
The lectures with tutorials dedicated to incompressible flows and incompressible flows with particles are available on GitHub: https://github.com/unicfdlab/Trainin...HDFoam-OFv1912
HPE likes this.
mkraposhin is offline   Reply With Quote

Old   August 5, 2021, 03:01
Default
  #3
Y.H
New Member
 
TANG YI HSIN
Join Date: Nov 2020
Posts: 4
Rep Power: 2
Y.H is on a distinguished road
Hello, Mr. Kraposhin,
After reading the information about QGDFoam, I want to use this solver you develop to simulate some cases. However, I encounter some problems during operating. The following questions are which I want to ask:
1. According to The new OpenFOAM computational framework for fluid flows based on regularized equations, it tells me that the default value for alpha QGD is 0.5, ScQGD is 1, to set custom values, create files “alphaQGD” and “ScGQD” in the folder “0/”. If I do so, do I need to set the value of ScQGD in thermophysicalPreperties document?
2. How is QGDFoam work with turbulent models? I wonder if using QGDFoam to simulate turbulent flow, is there anything I need to be careful with? Or any specific steps are different from the operation which I implement when using rhoCentralFoam?

Kind regards,
Y.H.
Y.H is offline   Reply With Quote

Old   August 5, 2021, 11:53
Default
  #4
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 343
Rep Power: 18
mkraposhin is on a distinguished road
Hello, when you set alphaQGD and ScQGD in 0/ folder, values from thermophysicalProperties file are not used definitely. But maybe they are required for consistency.



The second question is interesting, because QGD equations are derived from averaging over small time-interval and therefore, they might behave similarly URANS/LES. On the other hand, the averaging procedure and rules are slightly different from Reynolds or Favre averaging and thus, a different system of equations is derived. I think, if we apply this averaging to URANS, we arrive to QGD/URANS approach with similar closure relations for Reynolds tensor.


For the QGD procedure you can refer to "Time Averaging as an Approximate Technique for Constructing QuasiGasdynamic and QuasiHydrodynamic Equations" by T.G. Elizarova DOI: 10.1134/S0965542511110078



I've used k-w SST + wall functions and other OpenFOAM models with QGDFoam and they have produced qualitatively similar to URANS results.






Quote:
Originally Posted by Y.H View Post
Hello, Mr. Kraposhin,
After reading the information about QGDFoam, I want to use this solver you develop to simulate some cases. However, I encounter some problems during operating. The following questions are which I want to ask:
1. According to The new OpenFOAM computational framework for fluid flows based on regularized equations, it tells me that the default value for alphaQGD is 0.5, ScQGD is 1, to set custom values, create files “alphaQGD” and “ScGQD” in the folder “0/”. If I do so, do I need to set the value of ScQGD in thermophysicalPreperties document?
2. How is QGDFoam work with turbulent models? I wonder if using QGDFoam to simulate turbulent flow, is there anything I need to be careful with? Or any specific steps are different from the operation which I implement when using rhoCentralFoam?

Kind regards,
Y.H.
Y.H likes this.
mkraposhin is offline   Reply With Quote

Old   August 6, 2021, 01:06
Default
  #5
Y.H
New Member
 
TANG YI HSIN
Join Date: Nov 2020
Posts: 4
Rep Power: 2
Y.H is on a distinguished road
Hello, Mr. Kraposhin,
Thanks for your quick reply. Your answer helps me a lot with my simulation. I will refer to your opinion on continuing my simulation. Thank you very much.

Best regards,
Y.H
Y.H is offline   Reply With Quote

Old   September 9, 2021, 03:43
Default
  #6
Y.H
New Member
 
TANG YI HSIN
Join Date: Nov 2020
Posts: 4
Rep Power: 2
Y.H is on a distinguished road
Hello, Mr. Kraposhin,
Recently, I'm testing tuning parameters of QGDFoam in the thermophysicalProperties document and encountering a question. There is a lot of information about alpha and ScQGD, but less about PrQGD. Therefore, I would like to ask about the relationship between PrQGD and other parameters.
I look forward to hearing from you.
Best regards,
Y.H.
Y.H is offline   Reply With Quote

Old   September 10, 2021, 10:07
Default
  #7
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 343
Rep Power: 18
mkraposhin is on a distinguished road
Hi,
normally, you shouldn't change value of PrQGD coefficient, because artificial heat conductivity is determined by artificial viscosity which is controlled by \tau parameter, which in its turn is already adjusted with ScQGD.



But if you want to adjust settings for the numerical diffusion directly for energy, you can change PrQGD. Or, if you want to simulate flows with wall heat flux, then you may need to set PrQGD to large values on walls.


I can also recommend you to read this paper: Elizarova T.G., Shil'nikov E.V. (2009) Capabilities of a Quasi-Gasdynamic Algorithm as Applied to Inviscid Gas Flow Simulations, J. Computational Mathematics and Mathematical Physics, 2009, vol. 49, No 3, pp. 532-548
where PrQGD was changed to 0.001 to reduce unphysical oscillations near discontinuity. The approach in the article is efficient, but it doesn't seems to be universal: you may benefit from it in one part of a domain and may loose some important features of your solution in another part of a domain.

p { margin-bottom: 0.1in; line-height: 115%; background: transparent }
Y.H likes this.

Last edited by mkraposhin; September 13, 2021 at 05:11.
mkraposhin is offline   Reply With Quote

Old   September 13, 2021, 03:09
Default
  #8
Y.H
New Member
 
TANG YI HSIN
Join Date: Nov 2020
Posts: 4
Rep Power: 2
Y.H is on a distinguished road
Hi, Mr. Kraposhin,
your answer helps me to have more realization about PrQGD. Thank you very much. At the present stage, I haven't considered heat flux yet. Therefore, I will follow your recommendation to keeping PrQGD equal to 1.

Best Regards,
Y.H.

Last edited by Y.H; September 14, 2021 at 00:11.
Y.H is offline   Reply With Quote

Reply
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
New CastNet release: FSI-coupling with OpenFOAM and CalculiX based on preCICE MartinB OpenFOAM Announcements from Other Sources 0 April 30, 2020 06:53
How to contribute to the community of OpenFOAM users and to the OpenFOAM technology wyldckat OpenFOAM 17 November 10, 2017 15:54
OpenFOAM 4.0 Released CFDFoundation OpenFOAM Announcements from OpenFOAM Foundation 2 October 6, 2017 05:40
OpenFOAM v3.0+ ?? SBusch OpenFOAM 22 December 26, 2016 14:24
New OpenFOAM Forum Structure jola OpenFOAM 2 October 19, 2011 06:55


All times are GMT -4. The time now is 07:52.