August 10, 2023 at 10:35 pmNguyen NguyenSubscriber
I am developing a transport diffusion model of nanoparticles to the brain consisting of 2 regions of white matter and gray matter. But I am having some issues with modeling diffusion through multiple regions in ANSYS Fluent. Can I have any guidance and support on this matter? Also, for boundary conditions, do I need to add anything extra for the meshing or we could just assign different multiphysics properties to each region and it should be good enough? Thank you in advance
August 11, 2023 at 7:57 amNickFLSubscriber
It is a little difficult to see exactly what you have in your model as the tree is mostly closed. But here are some things to think about.
– Use Named Selections. It looks like you have some defined already. You will want surfaces defined for inlets, outlets, important planes and also volume definitions for regions that will have different properties such as porosity, density, etc.
– It looks like you have some contacts between your bodies. This will help you identify the interface between the different “bodies”. Did you use the imprint option (in the geometry tool) to ensure the contact faces have the same bounds?
– If you want a 1:1 nodes across the bodies, as opposed to an non-conforming interface, then you will define these as a multibody part (again back in your geometry tool).
– I assume you are using the Patch Independent because this is coming from a scan or something that has lots of tiny faces, edges, etc. If there are edges that you do want to keep defined, you can put a Named Selection on them and the mesher will resolve these.
And a completely different thought, have your tried meshing this directly in Fluent meshing? It does pretty well with “dirty” geometry. Plus there are controls for proximity, so you have better control of how many elements are thru thin parts. If you are new to ANSYS Meshing, it may make more sense to move into Fluent Meshing and just start learning that tool.
A very interesting problem you have there!
August 11, 2023 at 8:22 amNickFLSubscriberOne more point, you may want to cutout a small volume where you can set an initial condition to. You could always try and do this with cell registers, but if you change the mesh the cells that are in the defined register may change and that complicates comparing simulations.
August 18, 2023 at 3:42 pmNguyen NguyenSubscriber
As I tried to model the brain matters as porous media and the transport of particles under diffusion through these regions, do you know how to do this on ANSYS Fluent?
August 18, 2023 at 8:05 pmNickFLSubscriber
So there is no advection of fluid into/out of the domain? If so, then it is simply a mass diffusion problem.
I would recommend you make a simple "learning" model, so we can test and debug the process. It could be a simple box (and if there is advection, a channel).
- In your domain, create a small domain where you want the initial concentration to be. In the case of our simple box, make the cutout somewhere away from center a bit closer to one of the faces. Have the volume of this be ~5% of the domain. (Note you could do this using the marking and registers in Fluent, but the downside with this approach is changing the mesh could potentially change the amount of initial concentration.) When creating the geometry, create it as a multibody part to have a 1:1 interface across the domains.
- Mesh it as before (are you using ANSYS meshing?). Create a Named Selection for the small domain.
- Create a transient simulation. The most important part is creating the multi-species mixture. Basically you will want a mixture that is the component, let me call it brain fluid, and a copy of this brain fluid, let me call it dye. The two components may have the same properties, and, if it is simply a diffusion problem, the most important part is the mass diffusion quantity.
- If it is only a diffusion problem, initialize the solution with zero velocity (if it has advection, then solve the steady-state problem to obtain the velocity field.) We will then patch the dye onto the small cutout we made. You can find this under initialization in the tree, then Patch... What you will want to do is patch the mass fraction of dye to be 1 in the small domain that we created. (Do not hit "initialize", as this will destroy the velocity field if not zero.)
- Create monitor points that we will monitor during the run. These can simply be the mass fraction of dye at points or across surfaces. Use your imagination and also think about what is relevant for your problem. You know it better than I.
- Solve the transient solution. Watch the monitor points you created above until the solution reaches whatever point you want.
Ok, so that is a general walkthru. I would recommend searching for residence time simulations or calculating the mixing time in this forum or elsewhere on the web for a more detailed description. It is a pretty common problem, at least as I understand it at the moment. Again, I could be making some false assumptions, so go through the thought process and let me know if you have questions. I am here (somewhere on planet earth with an internet connection), and will try to help.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Suppress Fluent to open with GUI while performing in journal file
- Mesh Interfaces in ANSYS FLUENT
- Time Step Size and Courant Number
- error: Received signal SIGSEGV
© 2023 Copyright ANSYS, Inc. All rights reserved.