[mkraposhin]

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

[mkraposhin]

The lectures with tutorials dedicated to incompressible flows and incompressible flows with particles are available on GitHub: https://github.com/unicfdlab/Trainin...HDFoam-OFv1912

[Y.H]

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.

[mkraposhin]

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.

Originally Posted by Y.H

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]

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]

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.

[mkraposhin]

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]

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.