I am trying to calculate flow of steam valve in Ansys CFX. Boundary conditions : at inlet - massflow rate and temperature of steam, at outlet - averaged pressure of steam; wall for all other faces ;relative pressure - 0.
After calculation i have that steam does not pass throught outlet. In solution log i have:"
****** Notice ****** |
" | A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 100.0% of the faces, 100.0% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: Outlet. |
| The fluid name is: Steam1. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. "
How could this happen ?
https://www.sciencedirect.com/search?qs=Ansys%20CFX%20placed%20a%20wall%20at%20outlet&show=25&sortBy=relevance
Hi,
CFX uses "artificial walls" being placed in an outlet boundary condition cross-section in order to prevent the fluid from flowing from the outside of the flow domain back into it. How that can be caused (in particularly in the early stages of a CFD simulation)? The most common reason for this flow behavior is, that the outlet cross section was placed in a region of a flow recirculation, i.e. not far enough downstream of the investigated flow configuration. In that case a flow recirculation region is cut by the outlet BC and fluid attempts to re-enter the flow domain with unknown fluid properties (e.g. unknown temperature and turbulence properties). CFX tries to avoid this by placing artificial walls at cell faces, where such a not desired flow recirculation at the outlet cross section arises.
With multiphase flows the most common reason is the initialization of the flow domain in an unbalanced thermodynamical state. E.g. for water-vapor flow the initialization might be specified such, so that all initially specified vapor content is suddenly recondensing in the fluid domain. Or applied high pressure leads to sudden compression of the vapor content in the flow domain. Both leads to a corresponding sudden reduction in multiphase flow mixture volume in the flow domain and corresponding backward flow into the domain through the outlet cross section. I could imagine, that this is exactly what happened in your simulation and which caused CFX to close the outlet boundary condition with artificial walls to 100%. Since this leads to a sudden pressure drop in the fluid domain, rarely the CFX solver can survive such an initial stage of the CFD simulation and divergence of the flow solver is most likely.
How to circumvent it? First option is the usage of the corresponding CFX expert parameter, which allows you to switch-off this CFX behavior, i.e. to forbid CFX to use such artificial walls at outlet. A possible, but not in all cases successful strategy. It is successful, if the simulation survives the start of the simulation and if in fully developed flow conditions there is no backward flow at the outlet cross section anymore.
The second option is to think about physical reasons in your simulation setup, why that backward flow at the outlet might occur and to e.g. change the flow initialization in your simulation in a manner, so that this flow recirculation or backward flow no longer occurs.
Hopefully this was helpful to you for your CFD simulation setup improvement.
Regards, Thomas Frank.
Thomas Frank , thank you very much for your answer !!!
You are solved my problem. I changed material for fluid domen from Steam1 (from IAPWS-97 Ansys CFX library) to Water Ideal Gas (from Standard Ansys CFX library) and i finally got the results.
Apparently,like you say, error cause was initialization of the flow domain in an unbalanced thermodynamical state.
Much later , I have fully understood what was wrong. I was trying to calculate superheated steam flow using Steam 1 IAPWS-97. But in meantime, if you look CFX Theory guide you will see that the Steam 1 IAPWS-97 is used only for subcooled water (fig.1). I just needed to chooce Steam 5 to solve my task using steam.
Thomas Frank Many thanks Prof. Frank!
Your diagnosis was on the mark!
Recently I have been working on a multiphase solid-liquid flow in horizontal pipe in CFX. I observed the following:
1. When my pipe length was 100D (D=pipe diameter), the solver messaged "placing wall at the outlet". Here I had used tetrahedral+prism meshing for full 3D pipe
2. Then I extended my pipe domain to 140D, and this time it worked smoothly. Again the meshing was tet+prism
3. However, when I replaced the mesh with ICEM Hexahedral mesh, keeping same L=140D, full pipe, I am receiving same error at the start of the solution, "Wall placed at the outlet...."
As you suggested, today I am going to use the "Expert parameter option to put off that condition by CFX" and will report.
However, if there is any other reason, could you please enlighten me on this?
I shall be eager to hear from you sir!
- Badges
- Science topic
- Similar topics
- Filing