Discussion Closed This discussion was created more than 6 months ago and has been closed. To start a new discussion with a link back to this one, click here.
Incoherent results for a basic laminar flow reactor (LWR) using Transport of Diluted Species
Posted 22 mag 2022, 19:34 GMT-4 Fluid & Heat, Computational Fluid Dynamics (CFD), Chemical Reaction Engineering Version 5.2a 8 Replies
Please login with a confirmed email address before reporting spam
Hello,
To simulate laminar flow reactors, I started with the simplest case. Straight tube, laminar flow, first order reaction, steady state. I used “Laminar Flow” and “Transport of Diluted Species” (only convection, no diffusion). Results for velocity field are fine, showing a consistent radial variation; however, the radial distribution of the reactant concentration is flat, as if it was a plug flow reactor (pictures attached). This result in not coherent with a laminar flow velocity profile.
Did anyone also notice this problem with “Transport of Diluted Species”? On the document about this interface, the mass balance is correct, but the velocity vector is defined as “the mass averaged velocity vector”. Average? https://doc.comsol.com/5.6/doc/com.comsol.help.chem/chem_ug_chemsptrans.08.007.html#1607055
Thanks
Please login with a confirmed email address before reporting spam
I would do the simulation in 2D axial symmetry, it would simplify the calculation. I do not think there is a flaw, the parameters just make that happen. Usually I first compute the fluid flow and use that in the transport node. Solution takes only a few seconds in an axial symmetry. Your mesh is also quite dense.
Please login with a confirmed email address before reporting spam
I would do the simulation in 2D axial symmetry, it would simplify the calculation. I do not think there is a flaw, the parameters just make that happen. Usually I first compute the fluid flow and use that in the transport node. Solution takes only a few seconds in an axial symmetry. Your mesh is also quite dense.
Hi Lasse, thank you for your reply. I am simulating in 3D because I want to model a helically coiled tubular reactor. I started with a straight tube to check model consistency. Since diffusion is zero, this LFR has segregated flow (microfluid with no mixing). Consequently, there should be a clear variation of concentration with the tube radius.
Please login with a confirmed email address before reporting spam
What I saw is that the reaction rate is so high that entire concentration is consumed within first centimetres. Because there is no radial concentration distibution in the inlet, it has no time to develop because the concentration is zero most of the length of the tube. At which lengths are your concentration distribution plots (slides)?
Please login with a confirmed email address before reporting spam
What I saw is that the reaction rate is so high that entire concentration is consumed within first centimetres. Because there is no radial concentration distibution in the inlet, it has no time to develop because the concentration is zero most of the length of the tube. At which lengths are your concentration distribution plots (slides)?
The original file 'Radial concentration distribution.png' is a slice at the middle of the reactor. A horizontal slice in the attached pic shows that concentration fall gradually from 1.0, and is around 0.4 in the middle (z=0.5 m). Mean residence time is 8s. Plug flow with k = 0.23 1/s would result in concentration of 0.32 at the middle and 0.16 at the outlet.
Attachments:
Please login with a confirmed email address before reporting spam
For comparison, I successfully solved the problem as 2D axisymmetric, Mapped mesh. Only interface used was “Transport of Diluted Species”, inserting expression for laminar velocity profile. Attached are pictures of the radial concentration profile at z = 0.5 (middle of the reactor), from the 2D model (coherent) and from the 3D model (incoherent). Maybe the problem is in the 3D mesh...
Attachments:
Please login with a confirmed email address before reporting spam
Problem solved when I changed the unstructured free tetrahedral mesh to a structured swept mesh (see picture).
Attachments:
Please login with a confirmed email address before reporting spam
Great! Meshing is, indeed, very important in fluid flow and electrochemistry when you need to calculate conc. gradients.
Please login with a confirmed email address before reporting spam
Hello, I bring updates after many tests. I simulated this 3D straight tube LFR using two meshes: free tetrahedral mesh and structured hexahedral swept mesh. Up to 5 million elements, both with 5 boundary layers. The heat exchange and reaction yield from the free tetrahedral mesh were INCORRET. I only obtained coherent results with the structured hexahedral mesh (quadrangular at inlet, then swept). This issue was also reported by Mansour et al. (2020). To evaluate mixing in laminar flow, they simulated flow in a helical coil using different mesh topologies. They verified that the free tetrahedral mesh strongly overestimated flow mixing due to numerical diffusion in axial and radial directions, which could not be eliminated even with extreme mesh refinement. The numerical diffusion was the lowest with the extruded hexahedral mesh because the cells were better aligned with flow. So, free tetrahedral is NOT recommended to model laminar tube flow. Mansour, M., Khot, P., Kováts, P., Thévenin, D., Zähringer, K., & Janiga, G. (2020). Impact of computational domain discretization and gradient limiters on CFD results concerning liquid mixing in a helical pipe. Chemical Engineering Journal, 383(September 2019), 123121. https://doi.org/10.1016/j.cej.2019.123121