CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   If ANSYS can deal with electriferous fluid ? (http://www.cfd-online.com/Forums/cfx/22644-if-ansys-can-deal-electriferous-fluid.html)

white June 2, 2006 06:22

If ANSYS can deal with electriferous fluid ?
 
I want to simulate electriferous fluid moving in the electric field.But I can not find the attribute of electriferous fluid!anybody can help me?how to deal with this problem?

Joe June 2, 2006 07:05

Re: If ANSYS can deal with electriferous fluid ?
 
I have no idea what an electriferous fluid is and a quick google didnt help much either.

Provide a link to a description of it and I will comment on whether it can be moddeled in CFX. Generally, CFX can model most types of continuum fluids ...

white June 3, 2006 00:32

Re: If ANSYS can deal with electriferous fluid ?
 
It is known that most solid surfaces obtain an instantaneous electrical charge when in contact with an ionic solution.For example, fused silica that is used commonly in the manufacturing of microchannels becomes negatively charged when it is in contact with an aqueous solution. Such a negatively charged surface will attract the positively charged ions (cations) of the solution. When an external electric field is applied on this system, the thin layer of cation-rich fluid adjacent to the solid surfaces will begin moving towards the cathode. This boundary layer-like motion will eventually set the bulk liquid into motion through viscous interaction. my question is how to simulate this process?thank you!

white June 3, 2006 23:37

If ANSYS can deal with this problem?
 
It is known that most solid surfaces obtain an instantaneous electrical charge when in contact with an ionic solution.For example, fused silica that is used commonly in the manufacturing of microchannels becomes negatively charged when it is in contact with an aqueous solution. Such a negatively charged surface will attract the positively charged ions (cations) of the solution. When an external electric field is applied on this system, the thin layer of cation-rich fluid adjacent to the solid surfaces will begin moving towards the cathode. This boundary layer-like motion will eventually set the bulk liquid into motion through viscous interaction. my question is how to simulate this process?thank you!


Stuart June 5, 2006 07:53

Re: If ANSYS can deal with this problem?
 
CFX, like most CFD software has a fortran user interface, which will allow an advanced user to define conditions that can be applied to the fluid. So whilst there is no specific fluid of that type (electriferous) you may be able to simulate the effect upon a fluid by applying fortran defined exressions ???

Joe June 5, 2006 08:18

Re: If ANSYS can deal with this problem?
 
CFX can deal with this sort of physical problem.

There are at least two required building blocks for this model:

(1) A representation of the (time dependant?) electrical field in the channel. This can range from a hardcoded field derived from a known analytical solution to coupling CFX with an external electrostatics/dynamics code. This last approach is similar to the well established fluid-structure interaction (CFD<=>FEA) (FSI) approach.

(2) Tracking the local non-uniform concentration of cations in the fluid. This is relatively simple. You would use a single phase background fluid to represent the bulk fluid (e.g. water) and a so-called "fluid component" to represent the local cation concentration. This class of problems are generally dubbed "single-phase multi-component" flows.

You would then represent the electrostatic force on the cations as a body force acting on the bulk fluid weighted by the local cation concentration e.g. Body force = component fraction * grad(E) * dVolume, where "component fraction" would be a direct representation on the molar cation concentration.

In principle, this sort of approach could be used to model this problem inside complex 3D micro-channels in a time resolved fashion.

I cant give you more specific advice as you have provided very little information to work with. In particular, you havnt been specific as to the ultimate goals of this work which will obviously have a major bearing on the extent of CFD modelling required and even whether CFD is needed at all.

I would suggest digging about for papers describing similar modelling attempts (e.g. scholar.google.com). Avoiding the pitfalls encountered by other numerical analysts can save a great deal of time and kick start your own work.

Should you, in fact, need to model the system with CFD, start simple and work your way up the complexity ladder e.g. Start with a simple 2D model and an analytical description of the electric field and progress from there ...

If this sort of modelling hasnt been undertaken before you will need experimental data and/or analytical solutions to validate your model.

You seem to be working in an unsteady vicous laminar regime with an incompressible liquid, make sure the model (eventually) reflects this.

Naturally you can utilise multiple superimposed time varying electric fields i.e. a base electric field generated by the negatively charged channel surface which would provide the initial conditions, followed by the application of the main external electric field which would begin to force the viscous interaction of the boundary fluid with the core flow.

Again, if you provide more details as to the overall objectives, geometry etc. you will be given more specific advice.

Robin June 5, 2006 11:46

Re: If ANSYS can deal with this problem?
 
Hi "white",

There is a beta Electro-Magnetic capability in CFX that allows you to solve Maxwell's equations. Fluid properties, momentum sources, etc. can then be modified/created based on this field.

The details are beyond the scope of this forum and involves beta capability, so I recommend contacting your CFX representative for further details.

Regards, Robin

white June 6, 2006 01:47

Re: If ANSYS can deal with this problem?
 
thank you all very much, I will accept your advise and try it.


All times are GMT -4. The time now is 16:09.