Hello, I have a problem with the velocity vector display of a case run using the species transport model for 2 fluids. I displayed the velocity vectors color coded in terms of species. That gives me a single color for a single liquid. But somehow...the flow does not look laminar at all! the fluids seem to have diffused with each other completely, so that what start out as distinct red and blue streams end up as a homogeneous green. I should not b getting such results considering i had enabled the laminar finite flow option in the species transport model right?..i even clicked on viscous model/laminar to make sure before i did the iterations! would u have an idea of wot i am doin wrong?plz lemme know. thanks!the flow rates are 10mm/s..and the geometry is in the mm range.

I think you missunderstand the mean of laminar flow and turbulent flow.

You can have instabilities in the laminar flow, oscillations, waves etc...

When you have two phases they can be mixed by the mechanism of the instability. Have a look in the kelvin-Helmholtz instability for example....

So if you do not want any mixing, then eitheir you have to perform a steady state analysis (not transient), or you can use a high surface tension if you use a VOF method.

thanks Kharicha. Is there an option to enable while setting up the species transport model to specify that i want a steady state analysis? how do i prevent mixing from occuring by using high surface tension-i mean, where can i specify this???pls lemme know!

High surface tension will not allow the formation of small droplets. But are you using a VOF method ?

no i am not using the VOF method..i dont even know what VOF is!!

Well, then I missunderstood....but you have two fluids? you use a multiphase model ?

ok..here's the problem description..i have performed an expt in the lab using two different colored dyes to flow thru 2 different inlets of a microfluidic chamber...when they meet, the interaction is laminar, and they still flow as 2 separate streams thru the length of the chamber. i am trying to simulate the same behavior on Fluent using a species transport model..NOT a mulitphase model..i just used water and a custom defined fluid with slightly different density as the 2 fluids of the mixture...but the display results show that the 2 fluids have mixed completely!

You gave the symptoms...here is the diagnosis...

your problem is due eitheir to (1)

"numerical diffusivity" which induces an excessif diffusivity in your species transport equation.

(2) a flow which should be steady but due to numerical errors the flow oscillates.

Both are due to the grid...

First of all, create a structured grid (hexaedars) avoid tetraedars (creates 1 but also 2). The mesh should be aligned with the flow. Use steady solver first. Desactivate the concentration equations, and start calculations with only the flow, with first order, then with second order scheme.

Verify that your steady flow is well defined specially near the walls.

Then we come to the concentration equation, verify that the the area where you expect the die is well meshed... At least 10-20 cells within the thickness of your die...This is specially important if you have a very diffusivity in your species equation....

perform also a steady computation with ONLY the concentration equation. Then all together with second order scheme.