April 2, 2020 at 8:30 pmMRMRSubscriber
I didnt find the solution for my problem in available CFX tutorials so I decided to try getting help here.
I'm trying to simulate a steady state nozzle air flow with "holes" in the side wall as additional inlets for methane combustion exhaust fumes.
A simplified solid is presented in a picture below.
In fluid domain settings I would like to use "Air Ideal Gas" for the main Inlet (invisible in the picture, rectangular face from the side of coordinate arrows). The next aspect is is to define exhaust gases for side Inlets (in red circle): I used stoichiometric data from methane combustion, so I chose from the material library data four fluids:
- CO2 Ideal Gas (Volume Fraction in Inlet Fluid Values - 0.095)
- Water Ideal Gas (Vol. Fraction 0.19)
- N2 Ideal Gas (Vol. Fraction 0.715)
All of them as continuous Fluids; ref. pressure = 0; Non Buoyant Model; Stationary; None Mesh Deformation.
And in Fluid Models I got the problems:
From ANSYS Help I got the information: In homogeneous multiphase flow, a common flow field is shared by all fluids, as well as other relevant fields such as temperature and turbulence.
In my model the exhaust gases are joining the air flow and it's not all mixed from the beginning. So I didnt use this option.
The second option: Homogeneous Model of Heat Transfer I also didnt use, but if someone could explain this to me I would be grateful. I included Viscous Work Term and Total Energy (due to Kinetic energy impact I cannot use the Thermal Energy model).
In Turbulence I didnt use Homogeneous Model neither and no combustion or thermal radation is considered.
I used the option "Fluid Dependent" Turbulence, so in Fluid Specific Models part I chose for all components SST Turbulence Model with automatic wall function.
And in the next part there is my biggest issue: In Fluid Par Models I have one "Mixture Model" Interphase Transfer with basic 1 mm Interface Len. Scale a basic Drag Coefficiend of 0.44 in Drag Force. None Mass Transfer is included. How can I properly specify Heat Transfer between each Fluid Pair?
Main Air Inlet - Static Pressure 0.18 MPa, Zero Gradient Flow, Temp 900C, Volume Fraction Air 1, rest fluids 0.
Inlet 2 and 3 on the both sides of the nozzle: Static/Total pressure will be calculated later, but I need to get an ejection of fumes into the nozzle; flow - normal to boundary and static temperature of 1300C. I will repeat the Volume Fractions for these Inlets:
- CO2 0.095
- Water Ideal Gas 0.19
- N2 Ideal Gas 0.715
- Air 0
Outlet Av. Static Pressure 0.11 MPa (Ref. Pressure = 0). Wall of the nozzle is heated, and its' fixed temperature is 1100C.
Wall Contact Model: Use Volume Fraction.
Archive file attached - "1".
April 3, 2020 at 6:57 amDrAmineAnsys Employee
You do need to Gas Mixture and not Multiphase Model. Just define a custom material with variable composition / fixed composition and use that material as your fluid.
April 3, 2020 at 6:57 amDrAmineAnsys Employee
Moreover ANSYS Staff does not look into attachments but others can do.
April 3, 2020 at 9:16 amMRMRSubscriber
Hello Amine, thank you for your answer.
I created the Fixed Composition Gas Mixture but in my Domain I still do have two fluids (air for the main Inlet, and Mixture for the Side Inlets) and due to this I still have this FLUID MODELS card with all "homogeneous model" options for Multiphase, Heat Transfer and Turbulence. When I will not use any of them I still have to define Heat Transfer (Coefficient or Nusselt Number or other) and Interface Len. Scae and Drag Force in Fluid Par Models part.
April 7, 2020 at 8:23 amMRMRSubscriber
Hello, does anybody have an idea how to specify this heat transfer coefficient (air vs exhaust methane fumes)?
April 8, 2020 at 11:07 amDrAmineAnsys Employee
So actually you require variable composition mixture including air.
April 8, 2020 at 2:25 pmMRMRSubscriber
Thank you Amine for you help and commitment. Unfortunately I have to admit, that I'm a bit confused and probably got lost.
When I choose variable composition mixture, I use Calorically Perfect Ideal Gases Material Group and beneath I choose Air, CO2, N2 and Water - all ideal gases.
Then I choose the thermodynamic state of the mixture as a gas. I left Mixture Properties and didnt touch them.
In the next step I chose my mixture as Fluid in my Domain - Model SST with Viscous Heat Term and in Component Models I have all my fluids.
Nonetheless I got an error "One constraint component is required for the component fluid models. When I change the option from "Transport Equation" to "Constraint" for one of them it disappear from one of the inlet boundary condition (in the main one or in the both side ones - depends which one I choose)
Could you explain me what does this constraint option stand for? I cannot find it in ANSYS help or even in any other forum cases.
As a reminder
- my main inlet is an air one where I choose Mass Fraction 1 for Air and 0 for the rest
- my side inlets are for combustion fumes, where I choose Mass Fraction 0 for Air and corresponding values for each fraction CO2, N2, Water
Thank you again Amine for all your answers.
April 8, 2020 at 5:11 pmDrAmineAnsys Employeeconstraint specie is the blast one which will get algebraicly as 1-mass fraction of all other species which would be solved via dedicated transport equations.
April 8, 2020 at 5:12 pmDrAmineAnsys Employeeusually one would make the most abundant specie as the constraint one.
April 8, 2020 at 7:32 pmMRMRSubscriber
Thank you again Amine for your answers, especially that time. Unfortunately I'm afraid I'm not sure how it will work in my case, sorry. Could you try to explain one last time?
April 8, 2020 at 8:29 pmDrAmineAnsys EmployeeDon't worry. You have 4 species or components. One of the them should be a constraint. One generally take the abundant specie (like air in wet air) as constraint.
Now at the boundary where air enters: you provide zero mass fraction for the other 3 species. This results in having mass fraction of air at that boundary to be equal to 1.
April 8, 2020 at 9:00 pmMRMRSubscriber
Thank you very much - I got it. The problem is even funny, because when I changed all the options you said CFX showed me 3 mistakes for each inlet that "Air Ideal Gas is included" and should not.. And all I had to do is to go to each Inlet boundary again and approve the changes - that's all, that was what the hole incomprehension was about..
Thank you again, now I will check what the simulation process will show me.
April 9, 2020 at 5:39 amDrAmineAnsys Employee
- 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.