Simulation des écoulements d'huile en configuration cavernes/fractures

 

http://www.arabianoilandgas.com/pictures/gallery/OG%20ME/owd3.jpg​

Team members

Nicolas SOBECKI: 3rd year student at ENSEEIHT INP Toulouse, fluid mechanics dept

Tingting HAN: 2nd year International master at ENSEEIHT INP Toulouse, fluid mechanics dept

Seif ZOUGGAGH: 2nd year International master at ENSEEIHT INP Toulouse, fluid mechanics dept

 

Supervisers

Eric CLIMENT: IMFT/ENSEEIHT INP Toulouse

Annaig PEDRONOIMFT/ENSEEIHT INP Toulouse

Bernard MONTARON: Schlumberger China Petroleum Institute
 


 

Karst reservoirs of The Tarim basin in the North West of China have been verified as an area of large quantities of oil and gas. Very few oil reservoirs in the world are constituted of a network of caves, instead of porous medium. Existing industrial simulators based on the Darcy's law are not practicable. Navier Stokes model is adapted but is impracticable as well due to the complexity of the caves geometry for the boundary conditions and massive calculation and data burden. The simulator currently developed by Schlumberger is based on no physics laws and need to be verified and accurate. The aim of this project is then to give different small scale cases of the oil and water flow and analyze the outlet oil flow rate and the ratio of oil recovery using commercial and research CFD software which are Fluent and Jadim.

 


 
 
 
 
 
 
 
 
 

Introduction

As the last task for students of HYdepartment, before the final internship, the BEI is a long project allowing last year engineer students to work together for six weeks on an industrial project. 

As a result of a mutual interest, our team has joined the SimKarst project initiated in 2012 by Pr. Han Pingchou, PKU, and Bernard Montaron, Schlumberger China. The ultimate objective of the Simkarst project is to design a 3D reservoir simulator that can make realistic multi-phase flow simulations (gas, water, and oil) in large (20 x 20 km) and complex cave networks made of thousands of caves distributed in 3D space and connected according to a given pattern.

This project is our contribution in order to reach the ultimate objective.

 

 

 

 

Industrial context

Our project have its sources at the Karst reservoirs of Traim Basin in Xinjiang Province, in China. The challenge of our industrial partner "Schlumberger" was to improve the oil production of  the karst reservoirs, giving birth to the SimKarst project.
 
    http://califia.us/Tarim/tbasinanddesert.htm                                                                http://en.wikipedia.org/wiki/Tarim_Basin                                                                              
 
 
Karst reservoirs of Tarim Basin in Xinjiang Province of People’s Republic of China have been verified as an area with large quantities of oil and gas.
 
Carbonate formations of Ordovician age buried at more than 6000-meters depth in Tarim basin contain complex cave systems full of oil and water that are being exploited by Chinese national oil companies: Petrochina Tarim Oil Company, and Sinopec North-West Company.
 
 
 
 
 
 
 
 
 
 
 
 
 
 
 
www.geocaching.com/geocache/GC43T60_karst-quest
 
Below the network of caves,  an aquifer constituted by a porous medium where water goes up by capillarity effect under oil.
 
When oil is produced from a well, water goes up from the aquifer and a large quantity of oil is blocked due to the complex geometry of the caves. Therefore, a multiphase flow simulator is needed to optimize the production.
 
Very few oil reservoirs in the world produce oil from caves. For traditional reservoirs the oil  is contained in the micro-porosity of rocks with typical pore size less than 30 microns. However, in Tarim carbonate oilfields the karsts form complex networks of connected caves, with some caves larger than 300 meters and height exceeding 10 meters.
 
Existing reservoir simulators applied in the oil and gas industry are designed to simulate fluid flow in porous media governed by Darcy's law. These simulators are not appropriate for simulating fluid flow in cave networks where Darcy's law does not apply. The ultimate objective for schlumberger is to design a 3D reservoir simulator that can make realistic multi-phase flow simulations (gas, water, and oil) in large (20 x 20 km) and complex cave networks made of thousands of caves distributed in 3D space and connected according to a given pattern.
 
Navier Stokes model is impracticable because of complexity of the cave geometry for the boundary conditions and massive calculation and data burden.
 
Bernard Montaron proposed to investigate the feasibility of using cellular automata technology for such a simulator. This is one important objective of the so-called SimKARST project at Schlumberger China Petroleum Institute (SCPI).
 
The first part of the project started in October 2012 with two PKU students that developed a prototype cellular automata software to simulate 2D flow of water and oil in a cell with a simple geometry.This Method which is not based on physics laws but several rules, for example, the oil blocks will always move upwards when the water blocks are on top of them. So this method needs to prove its accuracy.
 
 
Therefore, an experiment on a specific geometry was realized in summer 2013 by two Enseeiht students: Nicolas Sobecki and Thibault Moreau, to verify and assist the development of the simulator.
 
 
The simulator is still under development and more cases are needed to verify its accuracy.
 
The aim of this project is to provide simulation results with different geometry using CFD software.
 
 

Objectives of the project

This project is aiming to:

  • Make a research on the different methods and numerical softwares to simulate two phase flow.​
  • Using VOF method and level set method to simulate the experiment cases and compare Fluent and Jadim results with it.
  • Simulate two phase flow (oil and water) in different geometry:
  • Plot the outlet oil flow rate and the oil recovery ratio versus time and compare the results given by the two softwares and the different geometry​
  • Compare the CFD simulations with cellular automata simulations in order to validate the cellular automata.
  • Assist the team working on gas injection with geometry and allow them to explore the technique.

Numerical methods and softwares

Numerical methods

Common Numerical methods:

 

Moving grids

The principle of moving grid method is to relocate grid points from a fixed number of nodes to nodes concentrating in the regions of rapid variation of velocity, pressure, etc. For its application in multiphase flow, this method track the interface by grid nodes on the interface and move interface grid nodes by Lagrangian transport.

                                               

  

  • Represent phase interface by grid nodes on the interface.  
     
  • Move interface grid nodes by Lagrangian transport:

    ⇒ It can result in large grid deformations which will make re-griding necessary.


     
  • Successful for small interface deformations.
     
  • Topology changes difficult
     
  • Difficult normal interface movement (phase change).
     

Marker Particles

The particle method is a mesh less method. Material to be simulated in form of individual particles. It is applicable for low phase fractions. For example, solid particles in air (eg. coal particle combustion) or fluid droplets in air (eg. diesel spray combustion). The limitation is that numbers of drops can be huge, which would cause large computational cost. Or drops are typically confined to relatively small regions of whole computational domain.

  • It tracks phase interface by Lagrangian marker particles in a fixed grid.
     
  • ​Phase interface can be reconstructed by polynomials through neighboring marker particles.
    ⇒ phase interface geometry is very accurate (normal, curvature).
    ⇒need to keep connectivity information of markers.
    ⇒topology changes are difficult.

     
  • Normal interface movement (phase change) is challenging.
     
  • ​The method does provides sub-grid phase interface resolution.

VOF method

It is a surface-tracking technique applied to a fixed Eulerian mesh where the Navier Stokes equations which describe the motion of the flow have to be solved separately.
 
The method is based on the solution of a transport equation for variable ‘C’ (often also referred as indicator or color function) for the liquid phase.
 
                                              
Cij represents the portion of the area of the cell (i, j) filled with liquid phase  and the phase function χ :
                       
We have 0 < C < 1 in cells cut by the interface S and C = 0 or 1 away from it.
 

The VOF method doesn't explicitly track the interface, it reconstructs the interface based on calculate the volume fraction of fluid . The Color Function also cannot be solved easily. There are already several method to approach, different approach gives different accuracy,  the most popular is PLIC (Piecewise Linear Interface Calculate). In a 3D space, the interface can be described by nx+ny+nz=a.

nx+ny+nz

Level Sets

It is a tracking interfaces technique that makes computations on a fix grid without having to parameterize the interface. A new dimension is introduced to the case and define the interface as a level set of function G(x,y) which represent the minimum distance from each point to the interface.

Softwares

Comparison of the CFD softwares: Jadim and Fluent with experiments

We will compare the simulations with Fluent and Jadim with the experiments, which are movies of oil and water flow in a certain geometry with and without connectivity.

The valves can not be completely opened in the experiments, therefore we will see if respecting the ratio between the hole area and the total area of the valve will have an impact on the simulations.

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m)
1000; 800 0.001;0.01 0.025

  bottom valve closed bottom valve opened
equilibrium time (s) 36.7 19.3

The first simulation is made without ratio for the valves, here is a comparison between the VOF and level set method with the Jadim software.

$$\rho_{water} /\rho_{oil}$$ (kg/m3)
$$\nu_{water} /\nu_{oil}$$ (Pa.s)
$$ \sigma_{oil/water} $$ (N/m)
mesh size (cells)
mesh size (m)
1000; 800
0.1;1
0.025
70x88
0.35x0.44
VOF method on the left and Levelset method on the right.
 
 
VOF method with fluent (same parameters)
 

We have increase the viscosity 100 times to avoid numerical diffusion near the interface but the VOF method still present a lot of numerical diffusion and therefore does not show a equal equilibrium at the end: the iso-contour of oil volume fraction value of 0.5 is not at the same height at the end. The level set method does not show numerical diffusion and still has some problem on the wall, this problem comes from the code which is still developing currently at the IMFT and was firstly coded for bubbles.

Therefore we will continue the simulations with the level set method and try a geometry with ratio.

The results comparing fluent and jadim with the VOF method are the same on the flow versus time but fluent shows less numerical diffusion.

 

 

 

 

 

 

Bottom connected case

In this case, a simulation using level set method with a refine mesh with jadim is realized, for which the geometry is exactly the same with experiments,  the mesh is is refined, and the bottom of the equipment is connected.   

Mesh

$$\rho_{water} /\rho_{oil}$$ (kg/m3)
$$\nu_{water} /\nu_{oil}$$ (Pa.s)
$$ \sigma_{oil/water} $$ (N/m)
mesh size (cells)
mesh size (m)
1000; 800
0.02;0.2
0.025
280x352
0.35x0.44

 

Experiment                                                             Simulation with jadim-level set method

In the bottom open case, after the valve opens, the interface moves mainly  due to gravity as well as U tube effect, and finally reaches equilibrium, with the same flow pattern, oil on the top and water on the bottom.  It is observed that the equilibrium time to arrive the final steady state are similar with the experiment and  simulation, despite a difference in viscosity. Also, compared with the fluids movement during the experiment, in which the interfaces of water and oil rises or drops more steady.  With simulation with the method level set in jadim, more dispersed phase appears.

Bottom blocked case

 A simulation with a refine mesh to simulate the experiment bottom blocked case is also conducted.

$$\rho_{water} /\rho_{oil}$$ (kg/m3)
$$\nu_{water} /\nu_{oil}$$ (Pa.s)
$$ \sigma_{oil/water} $$ (N/m)
mesh size (cells)
mesh size (m)
1000; 800
0.02;0.2
0.025
280x352
0.35x0.44

Experiment

Simulation with jadim-level set

 

For the bottom close case, the movement is  mainly led by the density differences. The final flow patterns are the same for the simulation and experiment.  The equilibrium time to arrive the final state is  similar with experiment and simulation. The movement is similar, however, same with the bottom open case, more dispersed phase appears in the simulation.

Results analysis

In this chapter, different softwares and numerical methods, as well as the results,  to simulate the experiments are illustrated. In general, simulation with VOF and level set method both give a results where flow patten is similar with the experiments, although equilibrium times varies. 

With jadim, the VOF method shows serious problems of diffusion in the case viscosity setting is 100 times smaller than the original ones. The interface can not be clearly tracked. With level set, the interface can be tracked easily, despite lots of dispersed phase appeared. With fluent, the problem of diffusion is less severe. 

The level set method in jadim with blocks is settled  in the geometry,which is the case of the experiment, shows a closer results compared with the experiment when equilibrium time is concerned. The VOF method with fluent  using real parameters is considered a precise simulation, too. It is estimated if the geometry and the fluid parameters are set exactly the same with the experiment with fluent, an accurate simulation would be realized, regarding the flow patten in the system and equilibrium time to arrive the final state.

 

Simulation of oil/water flow in different geometries with jadim and fluent

Geometry one

 The first geometry is used to establish a simple model for a network of three caves, with water from the below aquifer and oil is displaced upwards, as shown in the following pictures.


                                                             

 
 

Simulation with Jadim

Real parameters:

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m)
1000; 800 0.001;0.01 0.025

It is observed a lot of numerical diffusion on the interface with the real parameters, therefore it is difficult to distinguish the two phases,. A large area of the simulation would have the volume fraction of oil around 0.5, which is impossible because oil and water are not miscible.

 This phenomenon can be explained by the fact that in a same cell small portion of oil and water are present, therefore the oil volume fraction can not be either zero or one.

To avoid this problem, several modifications can be done, including :
- refine the mesh or increase the time step, but this would increase the time of calculation
- increase the surface tension to avoid the emulsion of the fluid
-increase the viscosity to avoid the effect of the separation of the fluid in others smaller structures.

Firstly, the viscosity and the surface tension are increased in order to analyze if the results are the same as the one with the real parameter with the help of another software fluent.

The parameters of the simulation are:

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) $$ dt_{min}/dt_{max}$$ (s) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) mesh size (cells) inlet Re
1000; 800 1;10 0.487 1e-7; 1e-5 0.056; 0.025 0.2 0.76x0.44 122x88 10

 

initial state                                                                                                                                   final state
 
 
This simulation shows no numerical diffusion, with the post treatment, the outlet flow rate and the oil remaining and recovery ratio will be analyzed versus time.
For the outlet flow rate:
 
$$ Q_{outlet}=\frac{1}{n}\sum \limits_{i=1}^n \tau_i  v_i L_{outlet}$$
 
$$ratio_{oil-remaining}=\frac{oil_{initial}-Q_{outlet}t}{oil_{initial}}$$
 
$$ratio_{oil-recovery}=1-ratio_{oil-remaining}$$
with n: number of outlet cells
$\tau_i$ : oil volume fraction of cell i
vi: outlet velocity of cell i
$$oil_{initial}=\sum \limits_{i=1}^m \sum \limits_{j=1}^l \tau_{ij} S_{cell}$$
m x l: numbers of cells of the domain
$S_{cell}$: area of a cell
 
To plot the data, the dimensionless number is applied, the flow rate reference is $Q_{inlet}$ and the time reference is $t=\frac{S_{domain}-S_{obstacles}} {L_{inlet} V_{inlet}}$, which is the time for water to fill the domain.
 
 
 
 
We have flow rate conservation due to the incompressibility of the fluids, therefore when only oil flow out the inlet and outlet flow are equal, after the dimensionless time around 0.3, water begins to flow out, so the oil outflow rate decreases and a change of the gradient in the oil remaining ratio plot which increases because less oil flows out in time.
 

Simulation with Fluent

Same parameters as the simulation with Jadim

$$\rho_{water} /\rho_{oil}$$ (kg/m3)

$$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) dt (s) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) mesh size (cells) inlet Re
1000; 800 1;10 0.487 1e-3; 0.056; 0.025 0.2 0.76x0.44 122x88

10

 

 

The results are almost the same, the differences can be explained by the difference of the two codes the way to solve the equations are not the same.

The fluctuations observed on the outflow rate of oil are due to the bubbles of oil crossing the outlet.

 

Real parameters

$$\rho_{water} /\rho_{oil}$$ (kg/m3)

$$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) dt (s) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) mesh size (cells) inlet Re
1000; 800 0.001;0.01 0.025 1e-3; 0.056; 0.025 0.024 0.76x0.44 244x176

1200

Decreasing the surface tension would increase the emulsion of the fluid and more bubbles would be created.

Compare with the last simulation, the viscosity has been divided by 1000, the velocity by 10 and therefore the Reynolds number obtained is 12000. If  the same velocity was kept before the Re number would have been 120000, which give a turbulent flow. That is why the velocity has been multiply by ten.

Compare with the viscosity, the decrease of the velocity is negligible.

Therefore it is shown the influence of the viscosity comparing the two simulations.

Results analysis

Comparison of the two fluent simulations: effects of the viscosity.

The oil recovery is larger when the viscosity increases, because it creates big bubbles which are flowed out by water.

In oil industry, the chemical products are used to decrease viscosity in the case of porous medium reservoirs, which decreases the capillarity pressure and therefore helps oil to go up.

It is estimated in the case of the caves network reservoir, increase the viscosity with chemical products can be considered as a method of oil enhanced recovery ratio.

 

 

 

Geometry two

For the second geometry,the case of two caves of different sizes connected by a fracture is considered, with water injection from the bottom, thus oil is displaced towards the upside, as shown in the figure below.

The parameters such as Reynolds numbers, viscosity of the fluids, interfaces tension, as shown in the table below, will be varied to see the effects on the oil recovery, sweeping efficiency, distribution of the remaining oil,flow rate, etc. The CFD softwares Jadim and fluent, are used separately to simulate this case. The sensitivity of mesh density is also tested.

Simulation parameters

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) $$ dt_{min}/dt_{max}$$(s) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) mesh size (cells) inlet Re
1000;800 2;20 0.487 0.1e-7;0.1e-4 0.02;0.05 2 0.45*0.35 90*70 20
1000;800 2;20 0.487 0.1e-7;0.1e-4 0.02;0.05 5 0.45*0.35 90*70 50
1000;800 0.1;1 0.1;1 0.1e-7;0.1e-4 0.02;0.025 5 0.45*0.35 90*70 200
1000;800 2;20 2;20 0.1e-7;0.1e-4 0.02;0.025 2 0.45*0.35 360*280 20
1000;800 0.01;0.1 0.01;0.1 0.1e-7;0.1e-4 0.02;0.025 1 0.45*0.35 360*280 2000

 

 

Similation with jadim - coarse mesh

Firstly, a coarse mesh and real parameters of fluids  are applied to simulate the flow with VOF method by jadim software.

However, the simulation is not reasonable because the water and oil is mixed.  This could be caused by the high Reynolds number or the density of mesh. Therefore, the inlet velocity is decrease and the viscosity is raised for the simulation. 

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) $$ dt_{min}/dt_{max}$$ (s) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) mesh size (cells) inlet Re
1000;800 0.1;1 0.025 0.1e-7;0.1e-4 0.02;0.05 5 0.45*0.35 90*70 200

This time, the phenomenon of diffusion is not as severe. But the mixture of the two phase still happens.

Thus, to avoid the diffusion, we need to use:

-a higher value of viscosity (100 times) to avoid this situation.

-a refine mesh. 

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) $$ dt_{min}/dt_{max}$$ (s) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) mesh size (cells) inlet Re
1000;800 2;20 0.487 0.1e-7;0.1e-4 0.02;0.05 2 0.45*0.35 90*70 20
1000;800 2;20 0.487 0.1e-7;0.1e-4 0.02;0.05 5 0.45*0.35 90*70 50

With the viscosity of the fluids 1000 times of the initial values and Reynolds within 100, the calculation finally reaches convergence. Below is the initial and final state for the Reynolds 50.

 

Similation with jadim - refine mesh

As mentioned before, to solve the problem of convergence during calculation and test the sensitivity of results to the mesh density. A mesh of density 16 times compared with the former one is applied.

To achieve the above objectives, two group of parameters are used for the refine mesh:

A. A group of parameters same with one of those used for the coarse mesh, which is:

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) $$ dt_{min}/dt_{max}$$ (s) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) mesh size (cells) inlet Re
1000;800 2;20 0.487 0.45*0.35 0.2;0.025 2/5 0.45*0.35 360*280 20/50

 

B. The interface tension as initial values. Viscosity 10 times and 100 times to the initial values.

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) $$ dt_{min}/dt_{max}$$ (s) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) mesh size (cells) inlet Re
1000;800 0.01;0.1 0.025 0.1e-7;0.1e-4 0.02;0.025 1 0.45*0.35 360*280 2000
1000;800 0.1;1 0.025 0.1e-7;0.1e-4 0.02;0.025 1 0.45*0.35 360*280 200

 

When the viscosity is 10 times, the problem of convergence still exists. However, for the case where viscosity is 100 times, the calculation achieves convergence.  For the group of parameters same with one of those adopted with the coarse mesh, the calculation converges; however it take almost 14 times to finish the simulation.

For case B, the movement of the fluids is similar with what we have obtained from the coarse mesh. Also, the interface between the two fluids is clearer.

 

 

Geometry two - simulation with fluent

To compare the differences results given by fluent and jadim. Firstly, same parameters with one group which is adopted by jadim in utilized, as shown in the table below.

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) inlet Re
1000;800 2;20 0.487 0.02;0.05 5 0.45*0.35

50

 

With fluent, we have more dispersed phase due to the high viscosity. The differences for the results of jadim of fluent will be discussed later.

Then the real parameters of the fluids is used to see the differences.

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) inlet Re
1000;800 0.001;0.01 0.025 0.02;0.05 0.066 0.45*0.35

1320

For the real parameters of the fluids, the viscosity is much smaller, the velocity is small, The weber number is very small, so the interface tension plays an important role in the process, so the interface does not change.

Post treatment and results analysis

1. Evolution of flow rate and oil recovery

In the very beginning before the dimensionless time reaches 0.3, the outlet oil flow rate equals with the inlet flow flow, because of mass conservation and that water has not reached the outlet. Afterwards, water reaches the outlet, the outlet oil flow rate starts to slow down, and the gradient for the oil recovery rate starts to slow down. 

2. Parameters sensitivity

A. Inlet Re

 

Re=20                                                                                Re=50

To evaluate the effects of Reynolds number on the oil recovery, all other parameters are set the same value except that the Re number are different at the inlet. For a high Re, water reaches the outlet earlier, and the value of oil recovery is higher. This could lead by the recirculation caused by a higher Re. 

B. mesh density (0.00125m/cell & 0.005m/cell)

 

Coarse mesh (Final state)                                                           Refine mesh(Final state)

From the figures of oil recovery ratio and flow rate, for the simulation with the refine mesh, the water reaches the outlet later, because the water diffuses less with the refine mesh. Therefore, we have a lower oil recovery ratio. And the interface in clearer with the refine mesh.  However, it take about 14 times to finish the calculation with the refine mesh. Thus, both calculation duration and the precise requirements should be taken into consideration when choosing the mesh density.

 

 

 

3.  Comparison for fluent and jadim

 

To compare the the differences of the softwares jadim and fluent, all parameters are set as the same value. From the figures, by using software fluent, water reaches the outlet with a shorter time. One possible reason is that there is more diffusion with fluent. Another reason for the difference could be the method used to calculate the flow rate at the outlet. In jadim, the oil outlet oil outlet velocity  is calculated by the average of the multiplication of the velocity and oil ratio in every cell by every time step. However, for fluent, this velocity is calculated by the average velocity and average oil ratio by every time step.

Geometry three

The third geometry is used to established a more complex network of three caves with several connectivity using ibm method (immersed boundary method) with jadim. The aim of this geometry is to discover whether oil would be blocked or water would be produced early .

$$\rho_{water} /\rho_{oil}$$ (kg/m3) $$\nu_{water} /\nu_{oil}$$ (Pa.s) $$ \sigma_{oil/water} $$ (N/m) $$ dt_{min}/dt_{max}$$ (s) inlet/outlet lenght (m) inlet velocity (m/s) mesh size (m) mesh size (cells) inlet Re
1000; 800 0.1;1 0.487 1e-7; 1e-3 0.5; 0.13 0.01 1.5x0.6 350x200 50

 

 

 

 

 

 

 

 

 

No oil has been blocked, but water begins to be produced at dimensionless time 1.3, where the curve of oil remaining and recovery ratio's gradients change.

Water production is not profitable for the industry, therefore "only" 80% of oil will be produced which is really important in comparison of the standard reservoir in porous medium in the world where the mean recovery ratio is around 35%.

Conclusion and perspective

Technical aspect

The method choice

The choice of the method for the simulation is of a clear influence, as we have seen with VOF/LEVEL SET for the experience simulation.
 

The VOF method is an adapted eularian method corresponding to our cases that aim for tracking the interface in limited geometry.

 

The code choice

One of the most tasks facing engineers is to choose the best simulation code according to the studied case.
 

For us the two candidates were Fluent and Jadim.

In our case the balance has tipped to Fluent, taking in consideration the approaching of experiment results for the equilibrium time. As well as it didn't present converging problems. One of the most important factors, is the the simulation time netly lower than the one made  with Jadim. Although it is important to mention the relative difficulty faced when changing and treating geometry.

Jadim has shown many advantageous points as the easiest way of managing geometry, and the high sensibility for phases that could be seen as diffusion while simulation. This high sensibility is not accompanied with a performance interface tracking which makes it a disadvantage for Jadim.

The commercial label of Fluent was also a factor of proposing Fluent as the accurate code for the project.
 

The geometry

We presented geometry with oil blocking possibilities as it occurs with karst caves. the sensibility of the oil blocked volume to the geometry is important.
 

Setting more complex geometry to approach real structures is recommended.
 

The obtained results will serve for the exploration of the gas injection part of the project.
 

Professional aspect

The project was an occasion to use some managerial tools for the project planning and the task dispatching. It was also an introduction of the team working conditions necessary for our near and far professional future.

References

[1] Bonometti Magnaudet Interferface Capturing CLS VOF

[2] Dominique Legendre two phase flow course

[3] DIRECT NUMERICAL SIMULATION OF FREE­SURFACE AND INTERFACIAL FLOW
Ruben Scardovelli1 and Stéphane Zaleski2
 
[4] SimKARST_experiment_of_two_phase_flow
Nicolas Sobecki/Thibault Moreau
 
[5] Two-Phase Flow Marcus Herrmann CTR.