

February 6, 2023 at 8:32 amYannik DannerSubscriber
I have a question about the setup for DQMOM PBM.
First I calculate (extern script) the six Moments for a PSD (lognormal). When i use "Load File" function in Fluent it prints out a possible inlet BC with 3 quadrature points QP0, QP1, QP2, exactly described in the Users Manual. But there are no steps described for setting BC. My expected proceding:
Given Length value is ~equal to particle diameter
Given volume fraction can be used to calculate inlet velocity or inlet vof
Given m4 > inlet m4.
the thing i am not sure about ist how to assign these valuese to my 3 secondary phases. is > QP0 inlet BC values for sec phase 1, QP1>sec. phase 2, QP2>sec. phase 3?

February 6, 2023 at 10:57 amDrAmineAnsys Employee
m4 is effective length. Once you have the information for three quadratures just provide the input (not really important what is QP0 or QP1) but afterwards after running one iteration check if the values will provide the expected PSD at domain inlet.

February 6, 2023 at 11:28 amYannik DannerSubscriber
Hey, thanks for the quick feedback.
Is there any documentation about the calculation of the Quadrature Points. Maybe there is a way to calculate them by myself or to split the PSD in my own way (to split PSD in predefined length (diameter) values)?

February 6, 2023 at 12:23 pmDrAmineAnsys Employee
Sure there is to get them caculated by yourself. You can refer to Moment inversion of Gordon and Wheeler. You just need to know that DQMOM is a direct quadrature and that is why different to QBMM or QMOM where the moments are required. So at the end you require for every qudarature point the moment to get size and volume fraction being calculated and from that the effective length is produced. The latter as well as the volume fraction information can be used as boundary input.

February 6, 2023 at 12:49 pmYannik DannerSubscriber
Nice, thanks for these information.
I am trying to simulate a bubble column via multiphase eulerianeulerian method in combination with inhomogeneous discrete or DQMOM population balance modeling. I am using 3 secondary air phases and a primary water phase.
Particle size range: (0.0015 0.0095 m). For the initial BC i wanna check three dfferent superficial velocities: 2.5 mm/s, 12 mm/s and 22 mm/s. I am calculation PSD extern with log. normal distribution to split the inlet velocity to the three phases (its recommendes to use inlet vof = 0.5 for inlet BC).
I tried to use these DQMOMmethod like u said. Cases with same operation conditions worked for QMOM and without PBM (3 and 1 sec. Phases). When using DQMOM simulation runs for low superficial velocity (2.5) at inlet. When using higher superficial velocity i get very high continuity residual (4.5475e+59) and floating point exception:
Stabilizing mpxmomentum to enhance linear solver robustness.
Stabilizing mpxmomentum using GMRES to enhance linear solver robustness.
Stabilizing mpymomentum to enhance linear solver robustness.
Stabilizing mpymomentum using GMRES to enhance linear solver robustness.
Stabilizing mpzmomentum to enhance linear solver robustness.
Stabilizing mpzmomentum using GMRES to enhance linear solver robustness.
Stabilizing k to enhance linear solver robustness.
Stabilizing k using GMRES to enhance linear solver robustness.Divergence detected in AMG solver: k Stabilizing vof2 to enhance linear solver robustness.
Stabilizing vof2 using GMRES to enhance linear solver robustness.Divergence detected in AMG solver: vof2
turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 4500 cellsError at host: floating point exception
Error at Node 0: floating point exception
Error: floating point exception
Error Object: #fSame Error while using inhomogeneous discrete method for same PSD. Is there something to consider in inlet BC spliting inlet velocity and volume fractions? I am not able to explain why discretization might be this mad for these setup when other velocitys or methods are running.

February 6, 2023 at 1:32 pmDrAmineAnsys Employee
DQMOM might be prone to numerical issues as the quadrature is dynamically updated for every cell and sometimes the problem gets so stiff. For that reaon I highly recommend that you continue experimenting first with inhomogeneous class method. If there you still have issues then you should revisit the way you are providing the bings and the closure laws.

February 13, 2023 at 3:27 pmYannik DannerSubscriber
Thank you for your advise. I could fix the Problem by using the gasvolumefraction instead of the inlet velocity for splitting the gasphase in 3 secondary phases!Now the calculation is running without errors.
I have another question with respect to the DQMOM inletBC. After using Wheeler momentinversion ANSYS gives abscissas(diameter values) and volume fraction + m4 (both calculatet from the weights and abscissas) for the inlet BC. When using m4 values for inlet BC simulation is running without problems but the sauter diameter from secondary phase is nearly similar. With this flow profile(velocities are similar too). I expect 3 different phases with different flow profiles and sauter diameter. Absciccas here where : QP0 = 13 mm, QP2 = 10, QP3 = 8 mm. PBM options max. Length = 10mm; min. Length = 1mm; reference Length = 6.3 mm
Sauter Diameter is very low in comparison with discrete and QMOM Method (6.7 ans 8 mm).
Is it really enough to give m4 and vof values from moment inversion for inlet BC to define the different secondary phases?

February 13, 2023 at 4:16 pmDrAmineAnsys Employee
From moments one can calculate the wieghts and lengths and from that the DQMOM nodes are evaluated. DQMOM is using dqmomm4 (effective length) and the VOF of the node as BC.

February 14, 2023 at 1:32 pmYannik DannerSubscriber
Hey, yes thats what I expect. Caclulating weights and lengths is meaningful.
This is my momentinversion:
QP0 QP1 QP2
Length (m) 8.542875e03 6.586689e03 5.078440e03
Volume Fraction 9.340751e02 3.345744e01 7.201864e02
DQMOMm4 (m) 7.979686e04 2.203738e03 3.657423e04I have 3 secondary Phases (Air1, Air2, Air3).
For BC is used: QP0 > Air1; QP1 > Air2 and QP2 > Air3 (volume fraction and dqmomm4).
When starting Simulation I expected that the SauterDiameter for each phase at the inlet is:
Air1 ~ QP0(length); Air2 ~ QP1(length); Air3 ~ QP2(length);
But all Sauter Diameter start at 0.001 m (thats what i defined the min Size). Its not even in the NDF what i used for inlet BC.
Why? how to define these diameter values? They are the essential values for calulating velocity.

February 15, 2023 at 7:43 amDrAmineAnsys Employee
You probably need to make the volume fraction input relative to the total "gas" volume fraction as stated in the Guide. Please check that on your side. For the initialization: are you using the values from Inlet. Please check that too.

February 15, 2023 at 8:26 amYannik DannerSubscriber
"You probably need to make the volume fraction input relative to the total "gas" volume fraction as stated in the Guide."
Thats what I do.
"For the initialization: are you using the values from Inlet. "
I will check that thank you.
I have another question, sorry.:
I saw that the Simulation gives Sauter mean diameter for regions with vof = 0, Sauter = 0.001 m = min. Length. Maybe thats not considered in global mean diameter and thats why its this low.
Do Ansys calculate the Eulerian velocity based on the Sauter diameter for each cell, or based on the global sauter diameter?
Sorry for dragging out this Thread but its good to have some help at this point.

 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.
Ansys Blog
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 Kepsilon and Komega Turbulence Model
 The solver failed with a nonzero exit code of : 2
 Time Step Size and Courant Number
 Mesh Interfaces in ANSYS FLUENT
 error: Received signal SIGSEGV

5290

3311

2471

1308

1016
© 2023 Copyright ANSYS, Inc. All rights reserved.