

September 4, 2018 at 8:21 pmrkoomulSubscriber
I am trying to solve the transport equation for a UDS (which is the number of particles, no units). The medium is stagnant water, so the convective term is zero. I have one boundary from where the particles are released, which is specified as number of particles released per unit area per unit time (which is the flux).
According to Chapter 8 of the Users manual, the boundary flux is specified as the diffusion coefficient multiplied by the normal component of the gradient of UDS. When we consider the units (say SI system), diffusion coefficient is kg/(m s) and gradient is (number per m). Therefore, the flux at the BC has the unit (number * kg/(m^2 s), not number/ (m^2 s).
What should be the units in which I need to specify the UDS flux at the boundary? In my case UDS is the number of particle.
Thank you in advance for your help.

September 5, 2018 at 11:17 pmjmccasliAnsys Employee
Hi koomullil,
I think the confusion here is for 2 reasons:
1) The governing equation for a Fluent UDS is an advectiondiffusion equation that is formulated with the fluid density multiplied throughout (see Equation 1.8 of the Fluent Theory Guide) . This is why Fluent's UDS diffusivity (let's call it gamma) has units of kg/(m s). Note that if you divide this by density, you get conventional diffusivity units of m^2/s.
2) It is not physically correct to say that your UDS (let's call it phi) is the number of particles. Since this is a field quantity that is governed by Equation 1.8, it must be (number of particles)/(unit volume), so phi has units of np/m^3 (where np is the number of particles).
It follows that the UDS flux, defined as gamma*grad(phi).n (where n is a unit vector normal to the surface) must have units kg/(m s) * np/m^3 * m^(1) , which you can rewrite as kg/m^3 * np/(m^2 s). Now you can see that the UDS flux value which Fluent expects from you is the number of particles per unit area per unit time, multiplied by the fluid density.
So to summarize, input the specified flux value as rho*np/(m^2 s), where rho is the density of the fluid, and np/(m^2 s) is the number of particles released from the surface per second, divided by the area of the surface.
I hope that answers your question.
Regards,
Jeremy

September 6, 2018 at 9:57 pmrkoomulSubscriber
Thank you Jeremy for the response. It makes sense now. I tested it on a unit cube, with quiescent water and a specified rate of release of particles from one of the sides of the cube. I did a transient simulation for 10 seconds. After the simulation, I calculated the volume integral of Scalar0 inside the cube and it is matching with the rate of release times the simulation time and the area.
The quantity that I am looking for is the number of particles that cross a given surface, say an interior boundary or a physical boundary. I couldn't find an option to do this. I tried surface integral of Scalar0, but it gives a large number because Scalar0 is the number of particle per unit volume. How do I calculate the actual number of particle crossing a surface?
Thank you,
Roy

September 7, 2018 at 7:50 amDrAmineAnsys Employee
As now you are dealing with a number density instead of the number you can imagine that the results for the discrete number would be mesh dependent. An idea to get the actual number is to define a custom field function where you multiply the number density with the cell volume and use that variable for further postprocessing.

September 7, 2018 at 1:45 pmrkoomulSubscriber
Thank you for the replay. Do you have any sample UDF which I can modify to calculate number of particles in each cell? The function that I am looking for is to define a new variable for each cell which stores the number density (Scalar_0) multiplied by the volume. Once I have this, I can calculate the average value of the variable on a surface.
Thank you.

September 7, 2018 at 2:41 pmDrAmineAnsys Employee
You do not require UDF. You can juste create a custom field function where you multiply your variable withe cell volume.

September 7, 2018 at 2:43 pmRobAnsys Employee
There are some examples in the UDF manual, and you may find some relevant solutions on the Customer Portal (https://support.ansys.com/AnsysCustomerPortal/en_us/Knowledge%20Resources/Solutions/FLUENT/328 looks like it might be useful).

September 14, 2018 at 2:09 pmrkoomulSubscriber
Thank you abenhadj. I created a custom field function and is working fine. Thank you for your help.
Roy

September 14, 2018 at 4:29 pmKarthik RAdministrator
Hello Roy,
I'm glad you're able to move forward with your work and are finding this community useful.
Just a small request: Students and other members of this community would benefit greatly if you could please mark the most useful response as a 'Reply' to your original question (once you are certain that your issue has been resolved). This makes it easier to search for solutions through these discussions.
Thank you.
Best Regards,
Karthik

May 27, 2020 at 2:53 am

 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.
Ansys Blog
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.
 Suppress Fluent to open with GUI while performing in journal file
 Floating point exception in Fluent
 What are the differences between CFX and Fluent?
 Heat transfer coefficient
 Getting graph and tabular data from result in workbench mechanical
 The solver failed with a nonzero exit code of : 2
 Difference between Kepsilon and Komega Turbulence Model
 Time Step Size and Courant Number
 Mesh Interfaces in ANSYS FLUENT
 error in cfd post

2706

2146

1357

1144

462
© 2023 Copyright ANSYS, Inc. All rights reserved.