Hello,

i have a problem where i have a microchannel with two inclined inlets with nano particles in fluid flowing through it. i am using a continuum approach. i have not yet considered the source term and have used only the advection term. I find that the concentration of the particles becomes zero after travelling a short distance. any help?

The other problem is, is there a way to avoid negative concentration in simulation. How to give a bound for the scalars particularly when reactions are involved.

with thanx sm

- How do you model the particles? Do you model them as real particles? If so, are they limited to travel over a fixed short distance or a maximum of 10 [s], which limits you?

- Make sure you will use Upwind as a discretisation scheme. However, this will gives you a lot of false diffusion. Be aware that the components can diffuse different from what you see in reality. Perhaps it is better to use High Resolution and use a source term like R=-k*max(0,C).

Gert-Jan

www.bunova.nl

Thanx Gert-Jan,

actually i tried increasing the physical time scale and could get a converged solution where i did not get a negative value for the concentration, but as you mentioned, the false diffusion was significant. Now i am using the high resolution scheme and hope the solution will improve. I was using max(0,C) for the source term when i was running it with the source term. as presently i am running it without the source term, my concern is to get a correct converged solution. Well , i am not using a multiphase flow. I am treating the particle concentration just as any other scalar.

when simulating for steady state , i was using a physical time scale of 10 s for the concentration of the particles. when i use smaller time scales, the convergence is poor. Basically, i am still not clear how does one select the physical time scale. The manual says for the fluid flow, it should be between 1/4 to 1/2 of L/U. can anybody say how does one select the time scale when there is a reaction?

Is it not a good idea to simulate for transient flow till it reaches steady state value so that the initial guess will be close to the solution and one need not worry about the physical time scale (using anyway a small time step)?

sm

Are the chemical reaction and the flow coupled? If not, you can switch off solving the fluids. This freezes the velocity field (Expert parameters; solve fluids = f). Then you only solve for the scalar, which reduces calculation time.

In general a larger time step, implies a more reliable solution, provided residuals are low (<1e-4), imbalance is 0, and values in monitoring points are constant.

What is the best timestep? Can you use a timestep which is 1/3 of your characteristic chemical timescale. With r=k*C, your timescale is 1/k?

Gert-Jan

www.bunova.nl

Dear Gert-Jan,

I am actually switching off the momentum equation. I just calculate once the velocity profile and use it for calculation of the scalar. I found that even with high resolution there is some amount of diffusion (switching off the source term). how can i avoid it? well my source term for the scalar is something like this. (no. per unit volume) x (no. per unit volume) x area x velocity x density. What should the time scale be in such a case. the residuals are all < 1e-4 and the imbalance is 0.0002% (without source term). Presently i am using a minimum time step of 0.01 s. with thanx

sm