January 27, 2023 at 3:17 pmAmirSubscriber
Description of the problem:
I am doing a 2D simulation on two droplets on a solid wall, the radius of droplets are 1mm and 0.5mm, the contact angle is 90, gravity were included (-y direction, i.e. to-down), however because of the size of droplets its influence is negligible. No other body force enforces on the droplets.
For two cases I am doing the simulation,
1) isothermal condition,
2) evaporation on the bottom hot wall with 5 deg higher than the saturation temperature of the droplet.
My mesh is fine enough to capture the droplets and in x direction is purposefully uniform.
The other three boundary conditions (up, left and right) are pressure outlet.
I am using
• Simple pressure velocity coupling,
• explicit formulation of VOF model
• second order discretisation for momentum and also for the case energy equation when is on,
• Geo-reconstruct for VOF,
• Presto for pressure ,
• Implicit body force option were activated.
• For the evaporation case, I am using lee model with different evaporation coeff.
Results and questions:
For the first simulation (without energy equation, without evaporation and in isothermal condition):
• droplet moves (oscillates) a little horizontally/vertically, which is tangible in the animation, which I don’t understand why?
For the second case (evaporation)
• droplets move a lot and in some cases even coalescence, while there is no temperature gradient on the wall, contact angle gradient, and mesh density in x direction, so it should not happen :(
Would you please some experts help me with this problem which is counterintuitive.
Thank you in advance.
For the first simulation (isothermal), the volume fraction contour in sequence,
For the secondsimulation (evaporation), the volume fraction contour in sequence,
January 30, 2023 at 4:25 pmRobAnsys Employee
Gravity is acting down, but the wall angle is 90 degrees. That may cause some issues. What time step are you using?
January 30, 2023 at 4:33 pmAmirSubscriber
thank you for your reply. I tried hydrophilic surface also e.g.,45 deg, but still droplet is not stable and moves.
the time step I chose is 1e-5
January 30, 2023 at 5:16 pmRobAnsys Employee
Try refining the mesh near the wall and lowering the time step. How well converged were the time steps?
January 30, 2023 at 5:25 pmAmirSubscriber
I took the adaptive time stepping with global courant number<0.2 for this case, fewer than 25 iteractions to be converged.
ok thanks, I thought the mesh size is ok, let me try a finer mesh near wall, I hope this problem will be solved
January 30, 2023 at 5:27 pmRobAnsys Employee
Turn off adaptive time stepping too. If the droplets are (mostly) stationary it's going to create some interesting numerical issues in the time stepping calculator.
January 30, 2023 at 6:19 pmAmirSubscriber
ok thanks alot, so you mean becasue the base of calcuation of time step in adaptive is based on cell’s speed,
when droplet is staionary evaporating and the numerically challeging phenomenon of mass transfer happens which need less time step to be captured,
but becasue of the low speed of the domain cells, wrongly the time step increase, and the physics is missed
am I right?
January 31, 2023 at 11:14 amRobAnsys Employee
More or less. When the physics is complex the adaptive time step adjustment can happen a time step or so after things have gone wrong - the function is great for "simple" systems where there are no sudden changes in a result. Here, it's going to struggle.
- 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.
- 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
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error: Received signal SIGSEGV
© 2023 Copyright ANSYS, Inc. All rights reserved.