Methane leakage to atmosphere question
 

Hello, I have several questions concerning a problem, which is completly new for me.

Problem description:
I have two 3D pipes. Each pipe is closed on one side and open on the other. Inside the pipes is a surface that represent a boundary between volumes (perpendicular to the length of the pipe) of air and methane (methane is on the closed side) - valve-like simplified representation. I have added a 3D enclosure around the pipes representing an atmospheric air volume. I want to perform a transient simulation of methane leakage from the moment of valve opening to see diffusion (concetration in the enclosured volume) of methane in the air-part of pipe and the atmosphere after given time. Methane has temperature of 20 celcius degrees and is kept at 4 bars of pressure until the valve is opened. Air is at standard conditions.

1. How to approach this problem in ansys fluent? Would you use UDF to describe decreasing in time mass flow of the methane as the pressure gets smaller?

2. Which solver should I choose - density based or pressure based?
3. Which models would you use? Maybe species transport + Realizable k-ebsilon turbulence model + energy equation?

4. Which boundary conditions would you use? (Enclosure external surfaces as far-field? valve-surface as pressure-outlet?



Can anyone recommend a similar case, that I can study and base my analysis on?


I would really any directions and any literature that would be of help. Thanks in advance!

Model Clarity
 

Your description of the geometry is not very clear to me. May be an image will explain it better. As far as leakage is concerned, you have to use ideal gas, until and unless the process is isenthalpic and you are interested in heating/cooling of methane. In the latter case, it has to be a real gas. Pressure based solver will work until the Mach number reaches 2.0. You can use species transport with and initialize the domain containing methane with 4 bar and mass fraction of 1 for methane. Pressure will automatically reduce as the methane will leak.

Thank you
 

Thank you for your help. Geometry in attachment: an enclosed atmosferic volume and a simple schematic of one of the pipe. The second one is similar but smaller and with a valve surface placed more in the middle of the pipe.

Geometric Model
 

As far as the objective is concerned, the model appears to be overdone. Until and unless the objective is to predict the concentration of Methane in the vicinity of the downstream ducts, all you need is a small sphere and the box around it with a small leakage hole connecting these two. Nothing else. Fill the box with high pressure Methane and the box with air at whatever pressure it ought to be at. Run the simulation in transient.

Thank you. Right, I made the enclosure too big, covering unnecessary space. A valueable remark!

The objective is to determine the methane concetration in air in vicinity of orifices after certain time. To be more precise, analysis will aim to determine space, where the concetration of methane in air around orifices will be higher than 4.4% (volume) fraction in any time. The volume of methane is finite and closed inside pipes. When the valves open, higher pressure (and other factors) of methane will cause flow of the methane through the pipes until it reaches orifices, pushing the air and diffusing into air in pipes, then flowing out of orifices mixing with air.

Volume Concentration
 

Species transport solves mass fraction and not volume. So, if you want to track on the basis of volume concentration, you have to define it. Secondly, gases have a fixed volume only at a certain pressure and temperature. When it leaks, it will no longer have a fixed volume. But mass is always fixed. You may not need to model any pipes, just the container and the leakage until and unless the leakage in the pipe occurs away from the container.

Thank you, I will consider a simplification of the model. When I manage to calculate it for the current geometry I will make another simple model covering the volume of the methane and the outlets to test it. In my opinion methane has high density in this conditions and the wall friction in pipes will influence the flow considerably and the methane concetration values in analysed time. Nonetheless, I will test what you are saying.



I have not made yet any analysis considering open-air models.
What boundary condition should I use at an enclosure surface in ANSYS Fluent?

Enclosure Boundary
 

If the enclosure is real, i.e., like a container or a room, then you can use wall boundary. If it is not real, like open atmosphere, then use pressure outlet.

Volume concetration
 

Thank you so much!

How can I calculate volume concetration of CH4 in each timestep having calculated solution already? Should I define it prior or post to solving the problem in fluent? Should I use UDF or is there any PDF already build-in in Fluent or other helpful functions/libraries.



Like you said species transport gives only mass concetration of the specified species. I couldn't find anything in Ansys Help neither could I find anything online. I just saw I idea of creating a loop over every cell in the sub-domain to calculate it. Is there an easier way to implement it?

Volume Concentration
 

Fluent solves for mass fraction of species, hence, volume concentration is not directly available. However, it can be calculated. UDF is not required. You can determine volume from the mass of each species. Mass of species is given by Integral of mass fraction. Then, the ratio of this mass and density gives you volume for each species.