# MHD BPISO etc

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

 January 10, 2005, 19:55 The first thing I must stress #2 Henry Weller (Henry) Guest   Posts: n/a The first thing I must stress is that I am not an MHD expert. I wrote mhdFoam one Sunday afternoon after buying a small book on MHD from the Imperial College library which looked interesting; it cost me 50p :-). What struck me most about the presentation of the B equation in the book was the similarity to the momentum equation so I decided to create an algorithm based on PISO to solve it. I have not read any papers on MHD or numerical solution of MHD problems so I have no idea if the approach I have taken is common or used at all, it just seemed like a good idea to me. My main aim was to create a method to solve both for the cell-centre B as well as face-fluxes for B as PISO does for U and apply the same kind of Rhie and Chow type approch to avoid staggering on a collocated mesh. This requires the solution of a "pressure" equation for B so I introduced a fictitious magnetic field pressure and used it to derive a flux equation from the div(B)=0 constraint. The consequence of this is that the fluxes exactly obey this constraint but the fictitious magnetic field pressure is non-zero, in fact it holds the non-convergence error which tends to zero as the system of equations are iterated to convergence. However, it need not actually reach zero, it will hold a form of discretisation error representing the difference between the magnetic field fluxes and the face-interpolate of the cell-centre magnetic field. Tests have shown this error to be small and hence the fictitious magnetic field pressure to be small. In conclusion the fictitious magnetic field pressure is only introduced to obtain an efficent solution algorithm. > Now, for compressible MHD flow BISO is unchanged because one > still wants div(B)=0, so I currently have a BISO loop in my > compressible MHD code that has the same form as the > incompressible BPISO loop. Will that be OK? That sounds correct although I am not sure what form the coupled term takes for compressible flow; does density not feature in the B equation at all? > Taking incompresssible PISO as a lesson on how to do all > this in FOAM, I would expect there to be a velocity > correction after the updating of the flux, as indeed there > is in the outer loop of ico-PISO. But in mhd-BISO there is > only a magnetic field flux correction That's because the fictitious magnetic field pressure does not feature in the B-equation and so cannot be used to correct B in the same way the pressure is used to correct U although looking at it now I think I could come up with a way. > no velocity correction follows. But the B-transport > equation is re-solved I don't follow you, where is the B-transport eqn resolved? > The question I have is: has this been analytically proven > somewhere to lead to an overall consistent segregated > solver? Nope, it was just my bit-of-fun on a Sunday afternoon which happens to work really well for the cases we have run. > Or is the BISO correction loop a seat-of-the-pants > rough correction attempt and not analytically rigorous. It's not analytically rigorous but more than seat-of-the-pants stuff; I do have quite a bit of experience with numerics and solution algorithms. > But then why is the coefficient "1.0/Ueqn.A()" used in the > BISO pBEqn for the correction to phiB? It should be 1.0/BEqn.A() but in fact for most cases they will be identical. However, for consistency I will change this. > A related question is does the "solve" on the "ddt(B)+..." > B-transport equation change the velcotiy field, which > afterall appears in that equation? No, it's a segregated solver. > Has the segregated solver emthod been > rigorously justified in these cases of multiply coupled sets > of equations, or am I better off waiting until an OpenFOAm > contributer delivers a robust block matrix solver set of OOP > features? Segregated solvers are fine and correct and efficient if they converge. Block-solvers are best for cases where segregated solvers either don't converge or convergence is very slow. Does the segregated solver not work for your cases? > Currently I'm thinking that for MHD I'll have to treat the > equations as explicitly solved (as a set) and therefore > requiring a strong CFL limit so that none of the coupled > fields gets too far out of synch on a given time step. Why do you think so? Why not try the segregated approach to see how well it performs for your cases? If you are worried about better coupling between the variables why not try putting an outer-loop around the equation-set. Henry amir.mofakham likes this.

 February 28, 2007, 04:27 Hi, I am trying to use the #4 mss Guest   Posts: n/a Hi, I am trying to use the mhdFoam and I have two questions: 1. What is the 'pB' ? 2. How I can impose 'dB/dx'? Thank you, Rita

 February 28, 2007, 06:22 Hi, Here are some precision #5 mss Guest   Posts: n/a Hi, Here are some precisions about question 2: It seems that the boundary conditions we can impose on the magnetic field B are only of Neuman type (B constant). Is it possible to impose a Dirichlet type condition (given rotational of B, or imposed current)? thank u, Rita

 April 27, 2007, 09:30 Hi everyone, First i would #6 New Member   Rui Alexandre Trigo Ribeiro Pereira Join Date: Mar 2009 Location: Coimbra, Coimbra, Portugal Posts: 23 Rep Power: 8 Hi everyone, First i would like to give my compliments to Weller and Hrv Jasak for their outstanding work in developing such a powerful (and extendable) tool as OpenFOAM. My main issue in this message is: 1) Would it be difficult to develop/implement a Solver for the compressible MHD CFD problem in a hot dense plasma, with radiation transport assuming a variable opacity (as a function of state vars in plasma) and multi spectral blackbody radiation? 2) What could be used as a coupling variable, between CFD and radiation transport process ( I assume the possibility of ocurrence of a Marshak wave in the problem) for the sake of numerical stability? 3) Does the moving mesh ability of OpenFOAM allows me to keep track of a boundary between two different media in case of the ocurrence of a Richtmeyer-Meshkov instability (in case of a cylindrical cumulative implosion problem, driven by MHD Lorentz force) or a Rayleigh Taylor Instability ( in case of a radiation shock dominated spherical implosion process, driven by an outer spherical shell ablation) ? Thanks in advance :-)

 November 5, 2010, 05:38 adding magnetic field in sonicFoam #7 New Member   giovanni silva Join Date: Jul 2010 Posts: 14 Rep Power: 6 Hi everyone, I am just a beginner in openFoam. At the moment, I am trying to add the term JxB in sonicFoam. I have seen that it is descriping by two terms -div(phiB,2.0*DBU*B) and grad(DBU*magSqr(B)) in MHDFoam which I put them in UEqn.H in my new Folder my_sonicFoam. I added the magnetic Field in creatField.H in OpenFoam/solvers/my_sonicFoam, DBU and #include "createPhiB.H" and I typed wmake and I have errors. I would appreciated if you could help me. Best wishes

 April 2, 2012, 09:53 USE OF LARGE EDDY SIMULATION IN mhdFoam #8 New Member   giovanni silva Join Date: Jul 2010 Posts: 14 Rep Power: 6 Does anyone know if it is possible to use LES ( LARGE EDDY SIMULATION ) in mhdFoam? Is there any tutorial? THANKS !

 November 14, 2012, 11:23 Lorentz force #9 Member   Lev Join Date: Dec 2010 Posts: 31 Rep Power: 6 Hello guys, do you know where can i find mhd solver with electric potential formulation that utilize Four Step Projection Method (for computing incompressible conducting flow at high Ha ) ?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

All times are GMT -4. The time now is 17:49.