August 28, 2018 at 9:04 pmmiguwhynotSubscriber
Currently I'm developing the simulation of the ascension of a high altitude ballon. It basically involves 2 different fuild volumes, one for the air and one for the helium.
You can see more details of the geometry model here: https://forum.ansys.com/forums/topic/meshing-low-thickness-region/
Or just check this images:
In my simulation the top cube face is considered as the inlet and the bottom face is considered as an outlet. So the air moves with a velocity of -4 m/s in the Y direction(see precious photos). Also inlet and outlet condictions changes with the time(as it get higher in the atmosphere) so a transient simulation is conducted(those conditions are set with UDFs) . When I implement the model in Fluent, I set ideal-gas model for both helium and air. You see, as the balloon gets higher so does its diameter (untill it finally burst) however, I don´t really know hot to set up that mesh with FLUENT.
I think it is dynamic mesh related but I'm not quite sure. Here´s some evidence of the Helium mantaining the exact same pressure during the whole ascendent move:
You can see in both pictures that the helium inside the ballon:
- Mantains the exact same size
- Maintain the same initial pressure
That results in a change in the thermal study which is my main purpouse of the simulation, so help its pretty much apreciated.
If you need any more information or have any suggestions please let me know.
August 29, 2018 at 7:37 amDrAmineAnsys Employee
To summarize you want to model the hull of the balloon becoming bigger as the pressure is reduced>Density is reduced>Mass is constant and that is why the volume of the balloon need to expand?
One possible way is modelling the hull of the balloon and using UDF to move the nodes to depict the volume change (DEFINE_GRID_MOTION). I am also thinking on using Mechanical and Autodyn here.
August 29, 2018 at 7:52 ammiguwhynotSubscriber
That's it! Sorry If my explanation wasn't clear enough, but what I'm having trouble is getting the appropiate conditions in order for the gas to change pressure. FLUENT shows me that the temperature does indeed change, that's why I though using the ideal-gas model (in materials properties) could be an option.
The main purpose it's to study the temperature change in the film of the ballon (im implementing radiation models and the obvious convection both natural and forced). I'm heading to read more about the DEFINE_GRID_MOTION, however if I'm to do it that way where should I implement the UDF?
Also I should probably have to read about how the diameter really change time dependant but I think this could very well be the solution. Thank you for your time.
August 29, 2018 at 8:44 amRobAnsys Employee
If you look through the tree on the left you'll see Dynamic Mesh about a third of the way down. I think you can do all of this in Fluent if you can assume the balloon can/will stretch to maintain the internal pressure.
More complex would be to either code a surface model into Fluent to adjust the balloon shape using stretchy laws (stress-strain: I'm a Chemical Engineer who does CFD). You may not need to go to a full FSI model.
August 29, 2018 at 9:18 amDrAmineAnsys Employee
I checked internally and I can confirm that is easier to deal with that with a structural solver if what is really happening in the balloon / on the balloon hull is not important.
August 29, 2018 at 10:47 ammiguwhynotSubscriber
Thank you both for your answer. I've been trying out the dynamic mesh and it seems a little difficult in my case.
To be honest, I think the volume change is not that relevant in my study, however I don't seem to be able to make a proper set up in FLUENT.
I'm going to try to give you as much information about my cell zones and boundary conditions and see if we can fix it.
- Start FLUENT load the mesh and activate, Energy, Radiation and Viscous (k-epsilon model).
- Set the top face as a velocity inlet, whose velocity is 4 m/s (that is the estimated ascension velocity) normal to boundary and the temperature will be set using a UDF that describes the atmospheric model
- Set the bottom face as a pressure outlet, whose Total Pressure will be set with another UDF.
- Set Helium and Air density to be estimated with the ideal-gas model.
- Set the ballooon film as a coupled wall with 0.002 m of thickness (shell conduction will also be an option in this case).
- Set gravity as -9.81 m/s^2 in the Y axis.
As it is I'm detecting a problem when the pressure inside the ballon starts to change. The material properties for the film have properly been set (so its radiation properties), when the solver starts, normally it haves some faces with back-flow in the oulet and limit some cells in the viscosity ratio.
I'm using pressure based solver, as atleast for the fisrt time-step (the only ones I can the the result) the temperature is more or less in the correct values.
I've already tryed to refin the mesh so the y+ would fit better without any result, so I think the problem is that I'm not setting up everything as it should, or that the solver doesn`t have the proper considerations on. In any case thanks again for your time and help, and sorry to bother you both.
August 29, 2018 at 12:16 pmDrAmineAnsys Employee
Which kind of problems are you now detecting I cannot follow. The settings you shared are okay. Which radiation model are you using and are you accounting for the incoming solar radiation? As you are activating gravity you need to give an operating density pointing to the outside of the domain. As you assume that your balloon is ascending and the op-density will also change with altitude I would rather put here a zero as reference and use atmospheric boundary condition at the the outlet (https://en.wikipedia.org/wiki/Atmospheric_pressure).
August 29, 2018 at 12:56 pmmiguwhynotSubscriber
Hi, thanks again.
I'm using the P1 Solar Radation Model, best to show with images:
Hi, thanks again.
I'm using the P1 Solar Radation Model, best to show with images:
Here's what I have at operating density and refference value:
In the pressure outlet here's what I have (the name of the udf doesn't matter overall it's just atmospheric pressure vs altitude made time dependant knowing the flight velocity):
The UDF is coded as follows having the U.S Standard Model (close to your refference):
The problem is that i can't seem to be able to solve the problem, here's what the console log looks like:
Thanks again for everything.
Edit: Uploaded case and data for more info: removed
August 29, 2018 at 2:59 pmDrAmineAnsys Employee
I won't be able to check your case files as ANSYS Stuff. Just a question: do you need a radiation model in your case? Why are you using explicitely P1 model (generally used for thick media).
Just help your self by debugging the case by switching off radiation, just applying the heat from solar radiation and paying more attention to the flow dynamic settings. Check the pressure resulting from your UDF. The pressure returned will be the static gauge pressure at your outlet (pressure-outlet). Reversal flow means that either it recirculate due to non-proper pressure field or it's physical. Turbulence is quite high at your outlet where I assume free-stream (stagnant flow) if the boundary is well far away..
Be aware this is an open community so everyone would might access your case. I will remove the link in your posting. You will then just share with the community members who wants to help you directly.
I hope the community will chime in here.
August 29, 2018 at 4:43 pmmiguwhynotSubscriber
Hi, Radiation is pretty much the thing I want to study, I though by setting up the P1 Model and the radiation propoerties will be the asier way for the solver (since the number of bands of 0).
It's true that radiation could be applied as a heat load. However i think my main problem is getting the flow with the conditions I want velocity, pressure and temperature. I have made myself a model with the exact same geometry, however radiation is off and only energy and viscous are on. It seems to work fine.
About the reverse flow happening, i think it´s mainly due natural convection, so I'm not worried that much.
I've been trying things out and it seems to me that the mistake is related to the flow settings. I'll keep trying I guess..
August 29, 2018 at 7:01 pmDrAmineAnsys Employee
Ensure for reasonable backflow quantities. Do not forget to initialize with hydrostatic pressure profile. Enable post processing of cell residual's under /solve set expert
August 30, 2018 at 8:47 ammiguwhynotSubscriber
Hi again. I've been making some test with a simpler geometry (only a cube without the sohere), and the problem seems to be the pressure outlet BC. As you can see I want the total pressure there to be set by my UDF (see previous message).
If I run the UDF with no sphere continuity seems to work just fine, but when I run it (with no other condition other than velocity inlet and pressure outlet) with a sphere in the volume the continuity ecuation doesnt convergen and I get the reverse flow message.
I think somehow my geometry isn't good what are your thoughts?
Edit: Even though I only have 2 different gas types, should a Multiphase model be applied?
August 30, 2018 at 9:09 amDrAmineAnsys Employee
No that is not a multi-phase case. Moreover the two fluids are not existing in the same domain. The pressure you are applying on the pressure outlet is static pressure whenever fluid flows out of the domain and as total pressure whenever it comes from outside into the domain. Continuity is always hard to converge for closed domains.
August 30, 2018 at 9:15 ammiguwhynotSubscriber
Hi, thanks again.
What would you suggest to make continuity converge? I get floating point error when I use the UDF, however if a constant Pressure is set (in the pressure outlet), FLUENT doesn't seem to have any trouble dealing with it.
I'm even considering making different steady simulations, since the transient seems to have that much trouble. But it really should be possible to make the transient case, since giving the values from the UDF as constant pressure it works just fine.
Edit: Using density solver seems to be helping
Edit: Still not able to run a proper set up, I think the problem could be the Helium not being able to change shape during the fligt. Since it changes density, using density solver reflects anormally high temperature in the film.
August 30, 2018 at 11:00 amDrAmineAnsys Employee
Your posts are quite confusing now. Please make a summary for all community members by starting from the Fluent case, cell zones conditions, materials used in each cell zone, models enabled, settings,..
August 30, 2018 at 11:36 ammiguwhynotSubscriber
Hi, okey I'll try to give a deep explanation.
Purpouse: Study the heat transfer during the flight of a ballon untill 32 Km of altitude. The ballon is supposed to move with a +4 m/s in the Y axis.
Geometry: - One fluid volume for the air and one fluid volume for the Helium inside the balloon.
- The air volume is a cube whose edge are 20R lenght.
- The balloon it's a sphere of R m Radius.
- Top cube face will be the inlet and bottom face will be the outlet.
FLUENT: - Time set to transient, since I'm going to simulate the temperature and pressure change with UDFs (code is shown in previous post).
- Air for the cube, helium for the sphere(cell zone conditions) and film porperties for the ballon skin (applied in wall menu).
- Velocity inlet (top face): Set velocity to 4 m/s normal to boudary and temperature defined by UDF.
- Presure Outlet (bottm face): Gauge Pressure defined by UDF(see previous post).
- Skin-wall: Set as a wall and asigned a thickness, shell conduction considered.
- Operating Conditions: Set gravity as -9.81 in the Y axis, Operating pressure as 0 and Operating Density as 0.
- Viscous Model k-epsilon and energy enabled (later on will try to implement radiation if able).
- Material properties for helium and air: desnity set by the ideal-gas model.
Problems: - When using Pressure Solver, not able to get any results.
- When using Desnity based Solver, anormally high temperature shown in results such as 500 K. When the max temperature expected is 288.15 K (could be more with radiation).
- In reality the ballon change its size during the fligh.
August 30, 2018 at 12:11 pmDrAmineAnsys Employee
Please disable Radiation first of all if still active. As the balloon is not expanding you will miss the cooling effect here (expansion cooling if one is far away from JT point). What about the sides of the cube: are there set to pressure outlet too or to symmetry?
Moreover: Setting the velocity inlet in a compressible flow is "lazy" as you may know this value but it's not the full boundary condition. Stagnation information for compressible flow are quite important. You can think about switching to either pressure inlet or to assume pressure far-field B.C on all cube openings.
You do not pressure-far-field B.C here a video of Raef using it for his Airfoil Tutorial
August 30, 2018 at 12:56 pmmiguwhynotSubscriber
Hi, thanks for your answer, the video was really helpfull. The side faces are set as Wall with zero wall flux, to be honest I'm not quite sure about this.
If I understood correctly I should set the far-field pressure in top and bottom face?
Edit: Radiation is Off
August 30, 2018 at 1:20 pmDrAmineAnsys Employee
Give it try! From the theoretical point of view when we give velocity inlet boundary condition for compressible flows, then its incomplete specification as density field is not specified. It may lead to oscillations & convergence issues due to incomplete specification at inflow boundary. You can use pressure farfield on all boundaries of the cube like in the video.
August 30, 2018 at 1:42 pm
August 30, 2018 at 2:29 pmDrAmineAnsys Employee
It would require further investigation and baby sitting of the all numerical methods and solution control. As ANSYS Stuff I cannot do more that I have already done here. I have highlighted some ways how to deal with that. Last comment:
1/You said without the balloon inside everything is working fine perhaps you need to investigate in that direction too. Try to setup a moving wall (the hull of balloon) without the helium being inside and check if it is working.
2/If using pressure-farfield the input for pressure and temperature has to be driven from the isentropic relationships. Your pressure profile and temperature profiles are the stagnation values.
I hope other community members may chime in here.
August 30, 2018 at 2:59 pmmiguwhynotSubscriber
Thank you for all your time and efforts.
- 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.