# Cfx emag

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

 February 4, 2010, 06:20 Cfx emag #1 New Member   Join Date: Dec 2009 Location: Berlin, Germany Posts: 5 Rep Power: 9 Hi, I try to simulate the electric and magnetic field around a current-carrying copper wire in air (concentric cylindrical domains) as a preliminary test for magnetohydrodynamic simulations. I use version 12.0 with EMAG beta-feature. 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.

 February 4, 2010, 09:52 #2 Senior Member     George Join Date: Mar 2009 Location: Birmingham, UK Posts: 257 Rep Power: 11 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. __________________ Top 4 tips 1. Knowledge is everything and Ignorance is dangerous. 2. Understand your limitations and try to eliminate them. 3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window. 4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials

 February 4, 2010, 10:56 #3 New Member   Join Date: Dec 2009 Location: Berlin, Germany Posts: 5 Rep Power: 9 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 non-zero velocities. Am I right? This would explain my problems with the current-carrying 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 EHD-module?? Thanks again

 February 4, 2010, 11:50 #4 Senior Member     George Join Date: Mar 2009 Location: Birmingham, UK Posts: 257 Rep Power: 11 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. __________________ Top 4 tips 1. Knowledge is everything and Ignorance is dangerous. 2. Understand your limitations and try to eliminate them. 3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window. 4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials Last edited by ckleanth; February 4, 2010 at 17:39.

 February 5, 2010, 03:20 #5 New Member   Join Date: Dec 2009 Location: Berlin, Germany Posts: 5 Rep Power: 9 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 zero-velocity field but without any magnetic quantities. That's why I thought it could work the other way round.

 February 5, 2010, 03:31 #6 Senior Member     George Join Date: Mar 2009 Location: Birmingham, UK Posts: 257 Rep Power: 11 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 __________________ Top 4 tips 1. Knowledge is everything and Ignorance is dangerous. 2. Understand your limitations and try to eliminate them. 3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window. 4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials

February 5, 2010, 05:48
#7
New Member

Join Date: Dec 2009
Location: Berlin, Germany
Posts: 5
Rep Power: 9
Hi, hopefully you are right

Here there are the model setup and ccl
Please tell me if there is something wrong
Attached Images
 geometry.jpg (32.1 KB, 84 views)
Attached Files
 model_ccl.txt (10.2 KB, 96 views)

 February 5, 2010, 06:07 #8 Senior Member     George Join Date: Mar 2009 Location: Birmingham, UK Posts: 257 Rep Power: 11 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. __________________ Top 4 tips 1. Knowledge is everything and Ignorance is dangerous. 2. Understand your limitations and try to eliminate them. 3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window. 4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials

 February 5, 2010, 08:10 #9 New Member   Join Date: Dec 2009 Location: Berlin, Germany Posts: 5 Rep Power: 9 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

 June 6, 2011, 10:19 2 phase flow #10 New Member   sarah Join Date: Oct 2009 Posts: 3 Rep Power: 10 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)

 Tags electric field, emag, magnetic field, magnetohydrodynamic, mhd

 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

 Similar Threads Thread Thread Starter Forum Replies Last Post Val Main CFD Forum 3 June 10, 2011 02:20 Ema CFX 4 August 7, 2009 05:39 Alphonso CFX 1 August 1, 2008 14:01 Rui CFX 9 May 28, 2007 05:59 Pandu Sattvika CFX 1 December 1, 2001 05:07

All times are GMT -4. The time now is 21:55.