August 14, 2019 at 1:21 pmkrndvSubscriber
I am trying to simulate a mixing tank with air sparging from inlet. The problem is set up as 2D- axisymmetric, Turbulent, Multiphase (Simple VOF) case. The system has an impeller for mixing, the phenomena is trying to capture using MRF technique.
1. Rotation is about X-axis
2. Inlet velocity is defined, Pure air is coming in so volume fraction of air kept as 1
3. MRF (around impeller) region is given -100 RPM using frame motion option.
4. The impeller wall is given moving wall (rotational) BC, with relative rpm with respect to adjacent zone (MRF zone) as zero.
5. Standard K-Epsilon Turbulence used.
6. Mesh quality - Minimum Orthogonal Quality = 9.98567e-01, Maximum Aspect Ratio = 1.487
7. Domian lenghth (along X axis) is 355 mm, in which up to 180mm is filled with water and above that air.
8. Interface defined between stagnant and moving zone
1. The problem is giving solution when solved in 3D.
2. Not converging with 2D axisymmetric set-up.
3. The problem has to be set up as 2D-axisymmetric or Axisymmetric swirl for capturing impeller rotation?
4. MRF technique valid with 2D Axisymmetric, multiphase case?
5. Possibility of using sliding mesh? (Tried and failed)
Hope some one can help me with answers for above question. Thanks in advance
August 14, 2019 at 1:21 pm
August 14, 2019 at 1:53 pmRobAnsys Employee
You'll need 2d-axi with swirl if you want the impeller to rotate, but have a think about the direction the blade will push the fluid. Also read up on the VOF model (including the theory) then explain why you chose it.
Bear in mind the difference between a 2d and 2d-axi case. Have you used the transient solver?
August 14, 2019 at 7:46 pmkrndvSubscriber
I have used Transient solver.Tried steady state, just got an oscillating residual, no stable result.
I will try with 2D-Axi swirl.
I was interested in getting just the volume fraction of air inside or gas hold up. So I thought simple VOF will be computationally less intensive as it solves one momentum equation for both the phases.
Thank you for your reply.
August 15, 2019 at 9:42 amRobAnsys Employee
VOF is a free surface model: it's perfect for tracking the water surface at the head space, but not designed for spargers. Read up on Eulerian and DPM then ask/explain your next steps.
August 15, 2019 at 3:54 pmkrndvSubscriber
What about carrying out the simulation with only water and degassing BC on top and air sparging from inlet? WIth Euler-Euler Multiphase model.
valid case set up?
August 15, 2019 at 4:39 pm
August 16, 2019 at 10:27 amRobAnsys Employee
Should be: I'd initialise with an estimated hold up volume fraction to help the solver.
August 16, 2019 at 10:58 amkrndvSubscriber
Ok, Thank you.
Could you please tell how to initialise hold up volume fraction?
Currently Im following the below given step
1. Steady state run for few iterations (10^-3 convergence of residuals) with no air input by giving sparger wall B.C and swintching off volume fraction equation.
2. After getting steady velocity of water domai - Switch on sparger(Mass flow rate inlet), volume fraction equation and transient run with time step of 0.01 secwith 20iterations per time step.
August 16, 2019 at 1:46 pmDrAmineAnsys Employee
You can initialize with certain volume fraction (standard) or use patch function to patch volume fraction in certain region of the domain. Please consider that degassing BC is only suitable for dilute dispersed flow.
August 16, 2019 at 5:52 pm
August 17, 2019 at 4:21 amkrndvSubscriber
1mm mesh used, quad dominant, inflation layer near walls.
METHODS- Pressure: PRESTO, Vol fraction: QUICK, First order upwind for all others.
August 17, 2019 at 7:14 amDrAmineAnsys EmployeeWhat about double checking the case and scrutinizibg velocity and relative velocity contours you can still model a sector of the whole tank with periodic conditions ?
August 17, 2019 at 9:12 amkrndvSubscriber
Thank you Amine.
You are saying about a 3D sector (Like 60 degree one) with periodic boundary condition?
August 19, 2019 at 1:51 pmDrAmineAnsys Employee
Yes if you want to save some cells.
August 19, 2019 at 4:18 pmkrndvSubscriber
Thank You Amine.
Tried and seems to be working.
August 19, 2019 at 4:20 pmDrAmineAnsys Employee
Great seems 2d axisymmetric has some issues here. Mark this as solved.
August 21, 2019 at 5:50 amkrndvSubscriber
I have one more doubt, while simulation a 60 degree sector I should use inlet flow rate (in kg/s) as actual one or 1/6th of actual flow rate.
August 21, 2019 at 6:25 amDrAmineAnsys Employee
For the sector modeled. I would rather use velocity inlet if you know the density at inlet.
August 21, 2019 at 6:34 amkrndvSubscriber
Yes its pure air coming in.
But the sparger got 7 distinct holes (per sector, 42 in full geometry) of 2.5mm dia, instead of drawing separate holes i made a slit of width 2.5mm with mass flow rate inlet B.C.
I will try with velocity inlet.
August 21, 2019 at 12:41 pmDrAmineAnsys Employee
Mass flow is always per sector in Fluent.
Yes. Have a fun. Please mark this as "Is Solved".
September 2, 2019 at 12:31 pmkrndvSubscriber
What is the technical difference between 'degassing' and 'pressure outlet (with back flow fraction = 0)' at the outlet boundary on a tank?
September 2, 2019 at 1:01 pmDrAmineAnsys Employee
Open new thread and I will tell you what is the difference if the documentation is not sufficient.
- 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.