August 7, 2018 at 8:31 amJimmyhanSubscriber
Hi, I am Jimmy. I try to simulate mass transfer in a slit. You can see my model geometry. This simulation focused on salt distribution. When flow cross this slit where at the up and bottom wall were membranes for separating the salt water (NaCl 35kg/m^3) in the main flow, I would like to know the salt concentration near the surface of the membrane. By the way, there is a quite small salt flux flow in the main flow from the membranes which we think as rejected salt. My question is that I have read the subsection 126.96.36.199 mass sources, but I still can not set the source and source coefficient. another question is for my topic should I set the source for the next step transport simulation, or use salt water directly and try to use some equation in CCL? Thank you very much!
August 7, 2018 at 11:30 amDrAmineAnsys Employee
A source is fully specified by an expression for its value .A source coefficient is optional, but can be specified to provide convergence enhancement
or stability for strongly-varying sources. The value of may affect the rate of convergence but should not affect the converged results.
If no suitable value is available for , the solution time scale or time step can still be reduced to help improve convergence of difficult source terms.
You can either work with multi-component flow and define the mixture as mixture of salt and fluid or you can solve salt as additional variable.
As ANSYS Staff member I cannot give you more support on this so that I hope that community members might pitch in
August 8, 2018 at 2:16 amJimmyhanSubscriber
Thank you for your explanation. Maybe I should try to use other ways. But can you give me some suggestion about the setting? If I use the subdomain as source what different between setting total model as the subdomain and adding new material? Furthermore, if I follow your suggestion the results from the mixture of salt and fluid are same as setting as salt flow, right? the periodic boundaries are necessary, right?
August 8, 2018 at 7:59 amDrAmineAnsys Employee
A simple multi-component approach (binary diffusion) would be similar to just working with additional variable. You have here the option to prescribe directly the mass fraction of salt in the mixture.
If your case is depicting a repetitive flow behavior (Gradient normal to the inflow/outflow boundaries of every variable except pressure is zero) then you can work with periodic boundaries
August 29, 2018 at 6:37 pmrgfsteedAnsys Employee
I'll explain subdomains first, but I think what you want is a surface source, not a volume source.
Subdomains allow you to apply a source across the entire volume of the subdomain. The "Source" option (units of [
/(m^3 s)] ) allows you to specify a local source as a field (which is integrated over each local control volume), whereas the "Total Source" option (units of [ /s]) allows you to specify a "total" source which is applied uniformly across the subdomain. If you need the source to vary across the domain, then use the "Source" option. Note that the units of the source also provide a hint as to what it's doing.
The source coefficient is only required if the source strength is a function of the current value of the variable for which you are providing a source. For example, if the salt source were a function of the concentration, then providing an expression for the first derivative (or a close estimate) of the source w.r.t. the concentration allows the solver to linearize the source (i.e. account for this change) when solving to improve convergence.
Sources at 2D regions
A 2D source can also be provided at any boundary. If your boundaries represent the membranes, then this is more likely what you need. On any boundary condition, visit the "Sources" tab to define a source. Once again, these can be provided as a locally varying field ("Flux" option with units [
/(m^2 s)]) or as a total source to distribute over the boundary ("Total Source" option with units [ /s]).
Note too that boundary sources can also be applied to the individual boundary conditions associated with interfaces.
August 31, 2018 at 2:06 amJimmyhanSubscriber
Thank you very much for your such patiently explanation. According to your suggestion, there are my questions:
- You must be logged in to reply to this topic.
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.
- 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 non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.