CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Thermal model with mass transport on seperate moving coordinate frame? (http://www.cfd-online.com/Forums/cfx/97275-thermal-model-mass-transport-seperate-moving-coordinate-frame.html)

evcelica February 13, 2012 19:06

Thermal model with mass transport on seperate moving coordinate frame?
 
Greetings,

This model is a bit above my head and I'm not sure how possible it is to solve, any help would be greatly appreciated.

I have the solution to a thermal fluid model, though will probably need to remodel to get this solution. (unsteady turbulent natural convection in an enclosure)

I am trying to find the distribution of ions that will generate in the volume and be absorbed by a ground plane. These ions will of course travel with the bulk fluid but they also have a drift velocity that must be superimposed on top of the fluid's velicity. (We are trying to avoid buildup of ions at any point where the fluids velocity is the exact opposite (or close) to this drift velocity, where molecular diffusion would then be the only path of shedding these ions. I'm hoping the turbulence will aid in distributing these ions.

The positive ion buildup would of course not affect the bulk fluid flow.
I am unsure how to superimpose the additional drift velocity of these ions onto the fluids bulk velocity. I must also make several boundary conditions walls where the positive ions are absorbed.

I am thinking I may be able to do this as multicomponent flow? Or use additional variables and a seperate coordinate frame for the ions? I've read through all the tutorials, and found some information, but I can't find one that applies completely to my problem.

Again any help would be greatly appreciated.
Thanks in advance,
Erik

evcelica February 13, 2012 22:51

So, I believe I can input my ion generation as a source term for an additional variable which I named "Ion Concentration." I can then add a diffusion coefficient sink the ions at any boundary by setting my additional variable to zero at those boundary conditions.

I just need to add this velocity to source to the ion concentration only so that:
velocity of the ion field = bulk velocity + Ion drift.

Can anyone give me any input on inserting this velocity source for the Ion field only?

ghorrocks February 14, 2012 17:49

If the ion drift has inertia you cannot use the additional variable approach. You may be able to get either an inhomogenous multiphase model or particle tracking model working, but neither of these models were developed for molecular scale objects.

But if your ion drift does not have inertia then think carefully about what is driving the ion motion. In this case is it not simply convection due to the fluid plus a diffusion? This is easily modelled with an additional variable.

evcelica February 14, 2012 20:00

Thanks for the reply Glenn, I really appreciate it.

The ion drift has no/negligible inertia. The ion drift motion is driven by an electric field of 50000 V/m, which I'm told translates to a positive ion drift velocity of ~8mm/sec for liquid Argon. I just have no idea how to add this drift velocity to my Ion concentration field along with the convective motion of the fluid, which I already know. Can you give me any pointers onto a way of doing this?

I've solved the model with a zero drift velocity just using a transport equation, but not with the drift velocity superimposed on the bulk velocity field.

Ansys support requested I do a electo-hydrodynamics model, but this seems much more difficult and unneccecary since I already know my drift velocity and shouldn't have to solve the extra physics involved. I know both velocity fields but i just can't add them together.

Thanks in advance

ghorrocks February 14, 2012 20:57

I cannot see how you can do this with an additional variable approach (but that does not say it cannot be done). It sounds like either you use an inhomogenous multiphase approach and you put a momentum source on the ion phase to get the drift velocity (and you have to tune the interphase drag to make the phases follow each other correctly but still have the right drift velocity); OR you use particle tracking and impose a drift velocity on the ion particles, but you still have an issue to tune the interphase drag.

evcelica February 14, 2012 21:37

Thanks for the options Glenn,
This definitely sounds like quite a lot more work than I hoped but I just need something to work. The inhomogeneous multiphase sounds like the one I'll attempt first, we'll see how it goes.
Thanks again!

cfdgremlin February 15, 2012 10:53

It seems to me that you should be able to model the ion transport separately with a transported Additional Variable solved on a frozen velocity field (solve fluids = f). This should be possible because the ions have no affect on the flow. The units of the additional variable would represent the concentration of ions in the fluid.

There is a feature in CFD-Post that allows you to overwrite field variables in a loaded results file with an expression (go to the Variables tab and select a variable to see this feature). This should allow you to superimpose the ion drift velocity on the existing (pre-solved) velocity field (e.g. velocity + mydriftvelocity).

CG

evcelica February 17, 2012 19:18

Thank you!!!!!!!,
I never knew you could do this in POST, I was searching everywhere in PRE. It makes sense that you cannot in PRE since it is not physically valid (it cant be inserted into a momentum equation) This seems like it should work, I'll try it right now.

I really appreciate your help and Glenn's, but it seems we don't have access to run multiphase, so this is my only option.

evcelica February 23, 2012 11:42

So I did this, and now I realize that it is still solving for the original velocity field, not my newly defined one. Is there something esle I have to do to get this to work?

I replaced velocity with my expression, which showed me new velocity vectors. I then went back to Pre and turned off fluids, turbulence, energy, and wall scale, but I set solve scalar to true. In solver manager I then just defined run based off current solution data. Should I use "Initial conditions" of that results file instead? When I tried that the solution blew up.

Thanks in advance
Erik

evcelica February 24, 2012 20:18

OK I got it to work, seems I just had to start from initial conditions and save it before I ran the new one.

Thanks for all the help everyone!


All times are GMT -4. The time now is 16:30.