July 12, 2018 at 1:04 pmInimsSubscriber
How do you select superficial velocity from the Flow Pattern Map of crude oil and natural gas in the case of simulating for slug flow. And what is the length/diameter of pipe require to generate this slug
Your help would be appreciated.
July 13, 2018 at 4:03 pmRobAnsys Employee
You need to decide what flow regime and boundary values to take from the Baker Chart and then apply those to the solver. You then add these conditions based on which multiphase model you choose, which is also determined by a combination of what you want to model and the boundary flow regime you choose.
Re the system length, this isn't a simple answer; it'll depend on speed and inlet conditions and may require additional interphase transfer terms coding in. I'd expect you to need over 30 diameters, and even then it's not an easy system to model. You may also struggle to resolve the flow within the 512k cell limit.
July 13, 2018 at 4:04 pmRobAnsys Employee
Just a brief note on posting, this may get more interest in the Fluid Dynamics section. I'll leave it here for now, but may move it on Monday.
July 13, 2018 at 4:52 pmInimsSubscriber
Ok. Hope discussion will continue on this
July 16, 2018 at 4:55 pmKarthik RAdministrator
I agree with everything said by rwoolhou.
I'd like to add a small note: I like to think about this problem in terms of mass flow rate as opposed to superficial velocity. Superficial velocity of the individual phases is generally prescribed in terms of the total inlet area. However, Fluent requires separate areas to prescribe the velocity inlet condition. Fluent uses these areas and velocities to calculate the volume flow rates appropriately. Irrespective of what area fractions you choose at the inlet cross-section for oil and natural gas, you have to calculate the respective phase velocities (to prescribe the correct velocity BC) such that they match the individual flow rates given by the Flow Regime map.
I just thought this piece of information might be useful in this thread.
Good luck with your model.
July 22, 2018 at 2:59 pmInimsSubscriber
Thanks for your contribution.
I'm starting with a 2D bent pipe of 50mm diameter. You mentioned Fluent requires separate inlet to prescribe velocities. Does that mean I should divide the inlet into two and specify ''gas inlet & water inlet separately?
July 22, 2018 at 3:02 pmInimsSubscriber
Thanks for your input.
Pls do I just pick corresponding values from the chart along the vertical and horizontal
July 22, 2018 at 3:38 pmKarthik RAdministrator
You should split the inlet surface into two when you create the geometry and assign respective named selections for gas and water inlets. You will see two surfaces in Fluent when you import this mesh.
Hope this helps.
July 23, 2018 at 1:09 pmInimsSubscriber
I did the flowing:
1] Geometry is a pipe component with 5cm outer diameter, 200cm vertical and 200cm horizontal with 90 deg bend
2] Splited the inlet surface(edge) into two halves and assigned Air-Inlet and Water-Inlet respectively.
3] The other end I assigned Pressure-Outlet
4] Setting up- general: Y(m/s2) = -9.81. Transient, Planer, Pressure-Based and Absolute were checked.
5] Multiphase model: Volume of Fluid, 2 phase.
Implicit Body Force, sharp and explicit (vol fractn formulation) checked. Phase interaction= (Surface tension= 0.072)
6. Turbulence model: K-Omega.
K-Omega model - SST
Materials: Air, Water
Operating pressure: 101325Pa
Operating density: 1.225kg/m3
7] Boundary condition: air = 10m/s, water = 2m/s, volume fraction for air at inlet = 1. I also tried vol fraction for air = 0.5.
8] Solution method = SIMPLE. I also tried PISO.
9] Solution control: Under-Relaxation Factors left as default
10] Residual monitor: Reduced convergence to 1e-06.
11] Initialised and Patch (note volume fraction: 0.5 or 1).
12] Run calculation: Time step size: 0.001 and 0.0001. Number of time steps: 1000 and 5000.
Summary: Did not generate slug flow. Global Courant Number greater than 250 always coming even after reducing time step.
Pls how can you be of help. Been running this simulation over the weekend.
I will appreciate your kind help and contribution.
July 23, 2018 at 6:36 pmDrAmineAnsys Employee
You can do a quick search on the net. You will see that for Two-Equations models and in order to mimic the reality, some turbulence damping terms on the free surface are required. Those terms will add more interfacial friction leading to slug generation.
July 23, 2018 at 10:32 pmKarthik RAdministrator
Are you running 2D or 3D simulations? Have you checked the quality of your mesh? Could you please share a few screenshots of your VF contour plots (or perhaps an animation)?
Another question for you - what is the y+ value you have used to generate the first thickness of your inflation layer? If you have not calculated it correctly and are not resolving your viscous sub-layer, you probably are better off with using a realizable or standard k-epsilon model with either a standard or a scalable wall function.
Hope this helps.
July 24, 2018 at 10:42 amRobAnsys Employee
The Baker chart will tell you which regime you're working in: you need to pick the boundary conditions!
This isn't an easy thing to simulate, and I agree with abenhadj as you may need to write a UDF.
July 24, 2018 at 9:30 pmKarthik RAdministrator
Another quick thought - you may want to go through the literature to find a similar study. Try to replicate the study and reproduce the results. It will help you build confidence in your model. It will also clarify a few things such as initial volume fraction etc. Initial volume fraction might impact the simulation results.
Hope this helps.
September 10, 2018 at 2:00 pmInimsSubscriber
Hi Kremella and All
I got some result in generating slug. See attached video.
However, I will need your kind support in creating results in Post Processing.
I can not find Flow-Time, PSD, Frequency and void fraction in the CFD-Post to plot my results.
How may you all help me.
September 10, 2018 at 3:24 pmRobAnsys Employee
Flow time should come from the data files, and volume fraction is also transferred. As you're using the VOF formulation there is no particle size and the frequency should be available via a Fourier Transform in CFD Post. I assume you saved data every some time steps through the simulation?
September 10, 2018 at 5:03 pmInimsSubscriber
I exported pressure, velocity magnitude, gas vol fraction and liquid vol fraction from Calculation Activities in Fluent. Though Flow time was moved along with the aforementioned variables but could not find it (flow time) in CFD-Post. I saved data every time step.
I will need direction for the FFT vs frequency, PSD etc.
November 13, 2018 at 11:06 amRobAnsys Employee
Sorry we missed this: it's a community so being away shouldn't matter as others may answer. As ANSYS staff we're also limited into how much detail we can go into. Your supervisor should be able to contact us, or via the University ASC, if a more indepth reply is needed.
Anyway, there is no PSD with the VOF model, although you could look at contours of volume fraction to see what sizes you're seeing. Re plotting the other variables, please review the manuals covering FFT etc as I don't think there's a tutorial covering this. Post should also retain the flow time, and it'll be a variable in the data: I always post process in Fluent as it gives me more options re the data.
November 13, 2018 at 12:27 pmInimsSubscriber
PSD is done in MatLab having obtain results in Fluent simulations.
I have decided to also Post Process in Fluent. I want to do XY plot for pressure, velocity and volume fraction versus flow time on these Axial Locations a,a0,b&c(attached). I just completed my simulations. Do I write to file? load file?...
Pls note, message can not be sent when I attached inline, hence I have attached it. Sorry if I ignore the rule.
Your support would be appreciated.
November 13, 2018 at 2:02 pmRobAnsys Employee
OK, so we can ignore PSD - what would be nice is if you could write a brief note on how you did that for the Tutorials section in case someone else want to do that. In return I'll look at the image.
Fluent stores data for each time step in a single file rather than all data as in the case of Mechanical. In your case all of the data is available, but not quite as easily accessed as you'd want. If I want that data I use a monitor during the run to save it out, and this is why when I teach the Intro course I always make a big deal about planning the simulations.
If the simulation is quick, then re-running with the monitors switched on may be quicker. Otherwise you can use a journal (I'd use the TUI) to read the data, report the values, read the data, report the values etc. To add the flow time to the text block you'll need (rpgetvar 'flow-time) which another user posted on here (the rest of that discussion isn't overly helpful). Use the TUI (text interface) to build the journal.
In the TUI, use
button to see what commands are available, and q to come back up a level. I'll get you started with:
The monitor data you want will be in Reports.
November 13, 2018 at 4:10 pmInimsSubscriber
I need to add the flow time.
The ''flow time'' is not coming up in both Fluent and CFD Post. This has been my problem all along. No journal file is coming up when I got to file > read > journal
This rpgetvar how do I go about it?
November 13, 2018 at 4:51 pmRobAnsys Employee
You need to write the journal to do this: it's not something Fluent produces during the run. If you type the (rpgetvar 'flow-time) command into the TUI in Fluent it'll produce the flow time. The data set you have is unique to that time step (instance in time): if you have saved many time steps then you have many unique instances in time.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- The solver failed with a non-zero exit code of : 2
- Getting graph and tabular data from result in workbench mechanical
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2022 Copyright ANSYS, Inc. All rights reserved.