July 16, 2018 at 12:57 pmmichele rocchiSubscriber
Both materials are defined as variable composition mixture; the material list for AIR is O2 and N2 and the material list for WATER is H2O and dissolved_O2.O2 and N2 are set as ideal gas. H2O and dissolved_O2 are set as liquid using the default property for water.
More in detail the material AIR is defined as: material group>user, mixture property>ideal mixture, thermodynamic property>equation of state>ideal mixture.
The boundary are:
An opening at the top of the column.
An inlet in the bottom region, where both AIR and WATER are introduced in the domain thought the throat of a jet ejector.
An outlet at the very bottom; the bulk mass flow rate is set in order to match the mass of water entering the domain trough the jet ejector.
The AIR that enter the domain is roughly 0.21 O2 and 0.79 N2 in mass fraction. The AIR composition at the opening on the top is set exactly in the same way, 0.21/0.79.
Mass transfer is right now set to none. My problem is that the mixture composition of AIR change throughout the domain with no reason at all, going from 0.00/1.00 to 1.00/0.00 O2/N2.
This happen completely at random: sometimes the composition remain constant at 0.21/0.79 for thousands of time step, sometimes some cell in the mesh change composition inexplicably, and once, after changing convergence control>length scale option from conservative to aggressive in the solver manager, in the entire domain the AIR changed in composition almost entirely to 1.00/0.00 O2/N2.
I hope someone can give me some explanation because now are few weeks that I’m tiring to understand the reason of that.
In the attached picture it can be seen a region close to the column wall where the mol fraction of
O2 in the material AIR change without explanation from 0.21 (the expected value) to something close to 1. Only a quarter of the column is simulated.
I thank in advance anyone that will be so kind to provide his opinion.
July 16, 2018 at 8:33 pmDrAmineAnsys Employee
Possible reason might be a strong backflow from the opening. Do not forget to enable buoyancy and set the density to the one of the continious phase. Moreover check if walls are created at your outlet. Moreover check for deep convergence in every single time step (by judging the variations of some Monitor points and flow imbalances). For post-processing do not forget to limit the visualization to the areas /regions where gas is present
July 17, 2018 at 10:44 ammichele rocchiSubscriber
I really apriciated your advice.
Actually the reference density was set to the one of the disperse phase. Thank you for that.
Walls are created some times at the outlet at the bottom of the column (20%-30%), the fluid that tend to "back-flow" is the disperse phase AIR. I don't have idea why AIR should back-flow from there; since the boundary is set as outlet I can't define the "fluid values" as for an opening. From a physical point of view, the column of liquid above the drainage hole should produce more than enough hydro static pressure to provide the required liquid flow at this boundary.
Do you mean that I should not care about the composition of the disperse phase in the locations where the disperse phase is not present?
I will monitor the flow at all boundary to see if this happens before the inexplicable change of composition.
I'm really grateful for your help.
July 17, 2018 at 11:31 ammichele rocchiSubscriber
I star again the simulation. in the picture on the right are evident some mesh elements where the oxygen concentration is close to 1 as indicated by their color.
However these elements are external to the iso-volume defined for AIR volume fraction larger than 1e-6 (picture on the left).
So probably I may assume that the
July 17, 2018 at 1:25 pmDrAmineAnsys Employee
Is the whole column filled with water or do you have a continuous puffer in the top (free surface). Regarding the walls which are created at the outlet perhaps is related to the pressure distribution.
July 17, 2018 at 6:54 pmmichele rocchiSubscriber
There is a free surface at the top.
I can avoid the free surface calculation (which I'm not interested in) if I use degassing condition for the opening on the top.
In that case I'm not allowed to set a pressure for the boundary. And I think this means that pressure in the domaine would be undetermined since there would be no other boundaries where I impose the pressure.
July 18, 2018 at 7:17 amDrAmineAnsys Employee
In that case then I would rather use the density of lighter phase as operating density and to initialize the pressure field with the correct pressure taking into account the hydro-static head (which is reduced by reference density time height time acceleration). Accordingly you have to set correct pressure definitions for your pressurized b.c's.
In case you work with degassing you still have an outlet and this would prescribe the pressure level. If you do not have any pressurized boundaries you can prescribe the pressure level information under Solver Control.
July 18, 2018 at 5:26 pmmichele rocchiSubscriber
I'm still using free surface and I put back the buoyancy reference density to the one of the lighter phase.
Now I add a short piece of conduit at the very bottom and I set the boundary to opening so that I specified the pressure and the fluid values: WATER volume fraction to 1.00 and AIR volume fraction to 0.00 with component details for AIR to 0.233 O2 mass fraction and 0.767 N2 mass fraction. (before the drainage was set as outlet and only the bulk mass flow rate was specified)
Regarding the fluid-dynamic I think the solution is pretty much converged. At least by seeing the gas volume fraction distribution in the column that remain stable over the time. The absolute pressure at the drainage, on the sparger and at the opening on the top (101325 Pa) are all three stable as well. Same situation for mass flow of WATER and AIR on the sparger at the drainage boundary and on the opening at the top of the column.
Checking the molar fraction of O2 at the sparger is 0.21 as it should be.
But again the domain does whatever it wants in terms of composition, I really don't understand and I'm a little bit contrariated about this. Now is quite some time that I can't get ahead of this. Below some screenshot in chronological order from left to right and from up to down.
You can see the molar fraction of O2 going from roughly 0.21 (at least in the region where air is present) to 0.00, then to values very close to 1.00, and then again some pockets at O2 molar fraction of 0.00 appears. I don't understand where that AIR with that composition come from (now all the opening are set as: component details for AIR to 0.233 O2 mass fraction and 0.767 N2 mass fraction).
Additional information that may be problematicin my setting are:
-the disperse phase is compressible (AIR is defined as: material group>user, mixture property>ideal mixture, thermodynamic property>equation of state>ideal mixture)
-At the sparger the volume fraction of water and air are set as zero gradient. This boundary is set as inlet>fluid dependent and then I specified separately the mass flow of AIR and WATER.
July 18, 2018 at 6:01 pmmichele rocchiSubscriber
Below are reported 2 plots for the O2 molar fraction in the AIR at the sparger location (areaAve(Air.O2.Molar Fraction)@Sparger) before and after the "compositional catastrophe". At the same time the color mapp on the sparger throat remain constant and fixed at 0.21 (first figure in the previous post low-right corner).
July 18, 2018 at 8:19 pmDrAmineAnsys Employee
Please create an expression where the mass fraction of oxygen is multiplied by the air volume fraction and define it as a variable for post-processing.
Specifying zero gradients is generally used for fully developed flows where the gradient of volume fraction normal to boundary is zero.
July 19, 2018 at 9:28 ammichele rocchiSubscriber
Here some sequential screenshots showing the product of AIR volume fraction multiplied by the O2 mass fraction in the air (Air.O2.Mass Fraction*Air.volume Fraction). On the very right are reported the AIR volume fractions corresponding to the first and to the last result.
Where the dispersion of air in water is present it is clearly visible a slightly change in the shade of the blue: from dark (first 2 screenshot) to lighter blue (the rest). Going from ~Air.O2.Mass Fraction*Air.volume Fraction=0.233*0.15=0.035 to ~1.00*0.15=0.15. On the top, where the AIR volume fraction is 1.00 it is clear the change in color from roughly 0.233 to 0.00 and then to 1.00.
I will calculate a the volume fraction at the sparger using the absolute pressure given by the solver at the sparger throat location and set the corresponding values rather than using the zero gradient option. I will also run a transient simulation hoping to see only 0.233 everywhere.
July 19, 2018 at 10:09 ammichele rocchiSubscriber
July 19, 2018 at 11:45 amDrAmineAnsys Employee
From the pictures it looks plausible in almost all parts. Bu If I look in the volume rendering screenshots I see in the top of column 100% O2 which is wrong if you are describing proper opening boundary conditions and you are working with proper density definition. How did you patch the top part of your column? Did you patch a air composition here?
I would moreover work on deeper convergence. The settings regarding components are okay. I think the results are fair enough. Perhaps one of the community member might add a comment here because as an ANSYS Employee I am not able to add more than I have already done without looking into the case directly
July 19, 2018 at 12:05 pmmichele rocchiSubscriber
May you explain how this can be plausible. I don't understand I'm sorry. I really don't get why the composition of AIR change completely at random when I imposed 0.233 O2 mass fraction at the only inlet boundary present in my domain. And when I monitor the area average AIR composition at the sparger boundary the molar fraction of O2 instead of remaining fixed at 0.21 it vary at random. As shown in the plot.
Could you please check those picture. Because as it is I can't do anything with a simulation where the material composition change at random when the mass transfer is turned off and the simulation is steady State.
Actually I realized right now that the images get compressed when uploaded and is really not possible to read anything
July 19, 2018 at 1:50 pmRobAnsys Employee
As abenhadj has noted, as ANSYS staff we can't be too specific with answers, and you may have seen us use forms of "unfortunately this question is the beyond the scope for ANSYS employees to answer on a public forum, so hopefully other student community users can chime in" elsewhere.
Having said that, the results do look odd if you have all of the phase material composition set at the sparger and top boundary: the gas volume fraction looks fairly sensible. So, check your settings, and also look at convergence as I can't think of a scenario where the gas would suddenly lose all of one component in normal operation.
Good luck with the project. Have you spoken to your supervisor?
July 24, 2018 at 2:55 pmmichele rocchiSubscriber
Dear Rob and Abenhadj,
I will talk with my supervisor next week.
For now I would like to gain a little insight in the main problem I had and still have:
The change in composition of a material without an apparent reason.
I think all the other small issues are much less problematic. It is obvious that I can't use a simulation where the composition of the domain vary over the time when all the boundaries are set in steady conditions.
After setting up a completely new simulation (from zero) in CFX-pre I have run a steady simulation and a transient. Both simulation are ok in terms of pressures and flows at the boundaries and at the monitor points. After reaching a more or less stable condition then again with no reasons the composition of the dispersed phase start to change both in the transient and in the steady state simulation. As I said the O2 molar fraction in the dispersed phase should be everywhere 0.21. This is the case for around 2000 step but than it change.
The only things I changed myself during the simulation were the flows before the1500th step (see link 3, 4, 5), in order to partially empty the domain from the continuous phase and to gradually (in stepwise manner) reach the final velocity at the sparger location.
I attach a link to a video showing the change in composition of the disperse phase:
. The video is relative to the steps between 2000 and 3500, the physical length is 1.46 minutes, and it is played 3 times.
O2 molar fraction in the disperse phase: video
It is clear that the composition of the disperse phase has the correct value of 0.21 molar fraction in all the domain but then some element positioned below the sparger location change to 1.00 and others to 0.00; after the inconsistency propagates to the entire domain.
Is there any reason for that? Any clue on what can be?
July 24, 2018 at 8:12 pmDrAmineAnsys Employee
August 3, 2018 at 4:58 pmmichele rocchiSubscriber
Right now in fluid specific model>component model, O2 is set as transport equation but kinematic diffusivity and turbulent flux closure are unchecked and the corresponding cells are empty.
This is the setting for both
-O2 in the dispersed phase material-mixture
-O2-solute in the continuous phase material-mixture
Does this make sense?
- 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.