Cfx emag
Hi,
I try to simulate the electric and magnetic field around a currentcarrying copper wire in air (concentric cylindrical domains) as a preliminary test for magnetohydrodynamic simulations. I use version 12.0 with EMAG betafeature. At the ends of the cylinders, boundary conditions (walls) are ground at the back side and a constant voltage at the front side, respectively, for both domains (domains differ in electric conductivity by a factor of 1000). The cylinder shell (wall) has constant temperature and zero flux for EMAG fields. The domain interface has conservative fluxes for heat and EMAG. The results for electric potential and field are ok but magnetic vector potential and magnetic induction look poor. Is there anybody with experience with electromagnetic modelling in CFX? Are there any special needs for EMAG simulation? I also did the same simulations for both domains solid with equal material properties except electric conductivity (again differ by factor 1000) and got no useful results. 
In studying the interaction between flow field and electromagnetic field, one needs to calculate the current density due to induction. There are two approaches are used to evaluate the current density. One is through the solution of a magnetic induction equation; the other is through solving an electric potential equation. CFX is using the first approach, and the magnetic induction equation is derived from Ohm's law and Maxwell's equation. note that current density in cfx is a vector
(if you have access) the fluent magnetohydrodynamics module manual describes this a little better. bottom line cfx will calculate j for you. in cfx coulomb and lorentz forces are included in the momentum equation but (at least this was true in V11) cfx would not calculate joule heat in the energy equation, and you needed manually to define the joule heat as a source term. However i think in v12 Joule heat is calculated automatically. if you dont need to know the temperature within the solid you dont need to model the copper, you can just as easy define a flux on the wall boundaries. try to check the boundary conditions on your problem, especially if you only have voltage/current in your problem obviously you need to apply the the electric field however all other wall boundary the electric and magnetic field needs to be grounded and you need to make sure that the zero flux option is used. another possibility is that you have not defined how the electric and magnetic flux transfer though your interface boundaries. 
Thanks,
I studied the fluent MHD manual. As far as I understand, it is only possible to calculate reasonable magnetic induction in cases of externally applied magnetic fields and/or the presence of fluid with nonzero velocities. Am I right? This would explain my problems with the currentcarrying copper wire in surrounding quiescent air without externally applied magnetic fields. Altogether, it is always necessary to have external magnetic fields involved in the problem and is therefore called MHD and not EHDmodule?? Thanks again 
remember cfd is all about solving the navier stoke equations.... if an electromagnetic field is applied near a dielectric/permeable fluid this will cause a momentum change because of the coulomb and lorentz forces so essentially your fluid cannot have zero velocities.
you cannot decouple the magnetic field with the electric field this is how the maxwell equations are solved, therefore whatever notation you use you will always solve the emag equations. 
I'm familiar with the coupling of electric and magnetic field, but obviously CFX cannot properly calculate the magnetic field when there is an electric field as initial physical field with an initial zerovelocity field but without any magnetic quantities.
That's why I thought it could work the other way round. 
I dont think the above is true and most likely you have a mistake with your BC and model setup.
post a picture of your setup and post the model ccl; perhaps then the probelm will be clear 
2 Attachment(s)
Hi, hopefully you are right :)
Here there are the model setup and ccl Please tell me if there is something wrong 
i think you did not ground the magnetic field. try to use Magnetic Potential = 0 [T m] on outer back boundary; if you want to get the magnetic field on the outer back boundary you need to add another domain and ground the magnetic field on that.

You were right,
I set Magnetic Vector Potential to 0 T m at the outer boundary and it now brings results comparable to analytical solutions for that configuration. Thanks again for your kind support and have a nice weekend, Marcel 
2 phase flow
Hi all,
I am trying to investigate the effect of EHD on two phase flow in a dielectric fluid  however the MHD model seems to be problematic for two phase flow and when I use the VOF model I am having problems with my UDS function to calculate the potential field. Has anybody done any simulations along these lines that could point me in the right direction? My geometry is 2D concentric electrodes (ground on outer tube) 
All times are GMT 4. The time now is 14:08. 