0

I am simulating Transport of Diluted Species inside a pipe segment in COMSOL Multiphysics. I have specified an initial concentration which produces a concentration distribution around a slice through the pipe at t=0. Moreover, I have a point probe a little bit upstream (I am using laminar flow for convection). I am plotting the concentration at this point dependent on time.

To investigate whether the model produces accurate (i.e. physically realistic) results, I am varying the diffusion coefficient D. This is where i noticed unrealistic behavior: For a large range of different diffusion coefficients, the concentration graph at the point probe does not change. This is unphysical, since e.g. higher diffusion coefficients should lead to a more spread out distribution at the point probe.

I already did a mesh refinement study and found, that the result strongly depends on mesh resolution. Therefore, I am now using the highest mesh resolution (extremely fine). Regardless, the concentration results still do not change for varying diffusion coefficients.

What could be the reason for this unphysical behavior? I already know it is not due to mesh resolution or relative tolerance of the solver.

Setup of the simulation: An initial concentration is defined at t=0 around z=1. Due to diffusion and advection (laminar flow) the initial concentration distribution is spread out through the channel. RX denotes the point at which I plot the concentration

Concentration at the point probe RX dependent on time. This plot does not change for varying diffusion coefficients D, even though it should.

Timo Jakumeit
  • 43
  • 8
  • Hey Timo, what diffusion coefficients are we talking about? Are we talking about gases (Schmidt numbers `Sc` of approximately `O(1)`) or liquids ( `Sc ~ O(1000)`)? What is the Péclet number Pe? It might be an indication that your Péclet number is high `O(1000)` and therefore the advection dominates over diffusion (generally the case for liquids). In that case the residence time distribution might not change much if you just change the diffusion coefficient by a factor of 2 or 10. Looking at your simulation I suspect this might be the issue and the simulation might be physical. – 2b-t May 27 '21 at 20:40
  • In such a case it would be good to have results to benchmark against but I guess for such a scenario it is hard to find any data. Have you only made a mesh refinement study or also varied the time step? Could you show results for different grid sizes and time steps to see if they are converging or not? Furthermore it would be useful to have more information about I) 2D/3D simulation II) grid size: number of cells, uniform grid, grid refinement III) time step. – 2b-t May 27 '21 at 20:45
  • Thanks for the suggestions. I'm talking about diffusion in liquids, in my case water. I have tried coefficients in the range of `D=1E-1` to `D=1E-25`. I have chosen the average flow velocity in a way that both diffusion and advection play a significant role (Péclet number `≈1`). My initial concentration is a relatively thin spike around `z=1`. The distribution at the receiver is smeared out, thus I am certain diffusion is having _some_ effect. Unfortunately changing the diffusion coefficient doesn't have any effect. – Timo Jakumeit May 31 '21 at 08:46
  • If I choose an arbitrarily small diffusion coefficient (e.g. around `D=1E-30`) the initial distribution should arrive pretty much unchanged at the receiver after some time, since it simply gets transported by advection and not smeared out by diffusion. This, however, is not what I observe. The distribution at the receiver is always smeared out. Could it be that the laminar flow interface in COMSOL is inherently adding some diffusion? Meaning that the _Transport of Diluted Species_ interface isn't the only source of diffusion? – Timo Jakumeit May 31 '21 at 08:46
  • Could you **add simulation type (2D/3D), diffusion coefficient, viscosity, characteristic velocity and length, grid size and the used solver** to the description. Please do not forget to add the physical units. Are you sure that you calculated (and set) the Péclet number? The Schmidt numbers for fluids are generally `O(1000)` and the Péclet number is given by `Pe=Re Sc` which means that already for low Reynolds number flows Péclet numbers are quite high and are advection-dominated. – 2b-t May 31 '21 at 17:20
  • Numerical schemes (can) have their own **numerical diffusion** but this should only be a problem in case the physical viscosity is very small. I have only observed that this numerical viscosity will smooth out very harsh gradients but I would not expect it to have an influence in case of a small Péclet number around `O(1)`. – 2b-t May 31 '21 at 17:36
  • Furthermore the distribution will always be smoothed out if you have a step function, a pulse or any other form of **discontinuity**. According to Fick's law the diffusion flux is proportional to the concentration gradient and therefore the time evolution is dictated by a Laplacian. For a step function at the discontinuity any derivative is infinite. This means already a small amount of diffusion - either of the physical medium or the numerical method - will result in smearing of the discontinuity. – 2b-t May 31 '21 at 17:45
  • I will soon provide what you asked for, but regardless of all these things, one thing confuses me: If I set the diffusion coefficient to `D=0`, there should be no diffusion at all. That means my initial concentration distribution should arrive unchanged at some later time downstream at the receiver RX, since it only gets transported by advection. However, I can still observe diffusion in my simulation, even for `D=0`. Why is that? – Timo Jakumeit Jun 01 '21 at 19:26
  • I would expect it to be caused by the **numerical diffusion**: Numerical schemes generally struggle with any sort of discontinuity as mentioned before due to having a discrete computational grid. Furthermore adding artificial diffusivity might make a numerical scheme more stable. You might want to have a look at [this](https://www.comsol.com/blogs/understanding-stabilization-methods/) if you have not seen it already. In Comsol they term this **stabilisation** and it is turned on by default for diluted species transport. – 2b-t Jun 01 '21 at 21:54
  • 1
    Any updates on this Timo or did you manage to resolve it by yourself? – 2b-t Jun 09 '21 at 22:26

1 Answers1

1

After a lot of time spent on this simulation, I concluded that the undesired effects are indeed due to numerical diffusion, as suggested by 2b-t. Of course, it is impossible to be certain that this is actually the reason. However, I investigated pretty much any other potential culprit in the simulation - without any new insights.

To work around this issue of numerical diffusion, I switched to Particle-Based Simulation (PBS) and approximated the concentration as the normalized number of particles inside a small receiver volume. This method provides a good approximation for the concentration for large particle numbers and a small receiver volume.

By doing this, I produced results that are in very good agreement with results know from the literature.

Nayana Chandran
  • 1,416
  • 1
  • 16
  • 30
Timo Jakumeit
  • 43
  • 8