Simulating of Fluid Sloshing effect inside a Gear-box

 Simulating Fluid Sloshing effect inside a Gear-box

AIM:

The primary objective of this challenge is to simulate the 'sloshing' of the fluid inside a gearbox. This challenge is to be carried out in Fluent using the Volume of Fluid method with help of User-Defined Functions (UDF) that generates moving mesh in the gearbox.

GIVEN PROBLEM:

perform the four simulations in the  Gearbox and then compare the results among all the four cases.

1. 20% Immersion, Fluid - Engine oil.
2. 30% Immersion, Fluid- Engine oil.
3. 20% Immersion,Fluid-n-heptane (c7h16).
4. 30% Immersion,Fluid-n-heptane (c7h16).

THEORY AND PROCESS:

To accomplish this we will use ansys fluent , so first open ansys fluent and load the geomety.

Then we have to choose the fluid volume inside the Housing. so select prepare-volume extract-edge select and select the respective edges and then click on the green tic .

 

Then uncheck the other volumes rather than the newly selected volume.

 

Now we have to split this volume into a 2d geometry so we will use split body command . Before that we go to design-plane select and select the middle point of x-y-z .

Then select split body - select the volume - select the plane - select the front body.

Then copy the face and in file- new design - paste the geometry. Before that select x-y plane by ctrl+6 then select the sketch mode below then paste the geometry.

 

Then cut the Design 1 so that we can work only with Design 2 , save it and import it further.

MESHING:

Then go to mesh - select element size 30mm - In sizing capture proximity-yes, promixity Gap factor-1 . Before that insert method- triangular because since the fluid domain consists of many curves and not straight-line geometries, it is best to use a tetrahedral mesh instead of hexahedral mesh (which may lead to inaccurate results).

 capture proximity is turned on because this allows us to capture small gaps within the geometry which makes the mesh more accurate.

We have to select name of the gears as left-gear and right-gear(while selecting the gears we have to be very careful as small portion mistaken can lead to dynamic mesh error at the fluent)

 Then update mesh close it and open set up.

SET-UP:

In physics  - General

select pressure based solver( because mach number <0.3)

select transient method ( as we have to deal with dynamic mesh and dynamic meshing allows the meshed geometry to change its position as per the time steps. )

select gravity on y axis as -9.81

select viscous model as k-epsilon,realizable with enhanced wall treatment ( as this particular problem does not involve analysing and inferring near wall effects, the k-omega SST model was hence not used.)

select multiphase as we have to deal with air as primary phase with engine-oil/n-heptane liquid as secondary phase, volume of fluid , implicit( volume of fluid method is used to track the surface between two immessible fluid and we use implicit method as using explicit method the courant number is becoming so large).

 Before choosing dynamic mesh we have to upload the c++ file of user defined function below.

so select User-Defined - Functions - compiled UDFs  - Add the file - Build - Load 

 Then select Domain - Dynamic Mesh - create/Edit - zone nemes - left gear , motion- left motion and right gear , right motion.Left gear centre(0,0) and right gear centre(0.115,0).

 Then Display zone motion and preview it so that to see if there is any flaws existed.

Then smoothing - Layering - Remeshing is used.

Smoothing - is used to adjust the mesh of a zone with a moving/deforming boundaies,the interior nodes of the mesh move but the number of nodes and their connectivity does not change.In this way interior nodes absorbes the movement of the boundary. Here we use diffusion based smoothing as it allows us large boundary deformation.

Layering - We use it to split or merge cells accross any moving boundaries.

Remeshing- When boundary displacement is large compared to local cell sizes , the cell quality can detoriate so to fix the issue we have to fix the sizes of the local cells.Load cell method is used only for triangular/ tetrahedral mesh.

max length scale-0.000118

min length scale - 0.0025

( to find out these numbers select mesh check in Domain zone and then in the console portion divide max/min cell volume by area.)

 

 Now we have to select the immersion portion . So to select it go to Domain - Adapt- Manage -Manage Adaption criteria - New - Autometic mesh adaption - cell Register - New - Region - Input cordinates - for 20% immersion y min upto -0.0475 and for 30% immersion -0.027 and name it as region_0( x=-1 to x=+1, Y=-0.0685 to y=-0.0475/ -0.027), then save and display.

 

 Then go to solution - initialize the solution as hybrid initialization (as the geometry has no inlet-outlet) 

Then we have to patch the region_0 with the geometry with the respective fluid engine-oil/ n-heptane.

 Now we have to show the mixing of two fluids air and engine-oil/n-heptane, so go to Results-contours-New and select like below

 

Then save and display

 

Then we have to create a solution animation of contour1 so go to solution-create- new animation and select contour-1 as animation .

Then we have to take the timestep size-0.0001 and iterations- 600( here gear rotation=200 rad/s so 200 =2*pi*f   & f= 31.83 cycles/sec . time required= 600*0.0001=.06 sec , so number of rotation cycle=31.83*0.06=1.909 or two rotations)

CASE-1(20% immersion in engine oil)

RESIDUALS:

 

VOLUME-FRACTION:

 

ENGINE OIL DENSITY:

 

VIDEO FILE:

https://www.youtube.com/watch?v=Kk1aKnO-3Xo

 

CASE-2(30% immersion in engine oil):

RESIDUALS:

VOLUME FRACTION:

 

VIDEO FILE:

https://www.youtube.com/watch?v=OKeDebyZmi4

 

CASE-3(20% immersion in n-heptane)

RESIDUALS:

VOLUME FRACTION:

 

N-heptane density:

 

VIDEO FILE:

 https://www.youtube.com/watch?v=14_YXxI4Dgo

 

 CASE-4(30% immersion in n-heptane)

RESIDUALS:

 

VOLUME FRACTION:

 

VIDEO FILE:

https://www.youtube.com/watch?v=S1aSyBAMJrU

 

CONCLUSIONS:

• It is clear from the volume fraction contours that engine oil is a far better lubricant as compared to n heptane.
• First of all, if we observe each and every tooth for the engine oil iteration, the volume fraction of engine oil is fairly uniform and shows a light blue colour everywhere.
• The simulation with n heptane as a lubricant on the other hand does not show a uniform colour (volume fraction of n heptane) distribution for all teeth.
• In some areas, light blue and green are the major colours and even in specific teethes, the volume fraction of n heptane is coming out to be very close to one.
• This indicates that the n heptane oil is getting stuck on specific teethes, thus not lubricating all teeth in a uniform fashion
• Hence, its concluded that engine oil is a better lubricant than n heptane.
• After analysing immersion rates, it was observed that higher immersion meant more fluid thus leading to better lubrication
• Hence, 30% immersion showed better and uniform results as compared to a 20% immersion of engine oil.

 What is Dynamic meshing? Give some other examples where dynamic meshing can be used. 

• Dynamic meshing is generally used to analyse problems where in several components are moving and not stationary
• Dynamic meshing capability is used to simulate problems with boundary motion, such as check valves and store separations.
• The building blocks for dynamic mesh capabilities in Ansys Fluent are three dynamic mesh schemes, namely, smoothing, layering, and remeshing.
• A combination of these three schemes is used to tackle the most challenging dynamic mesh problems.
• For simple dynamic mesh problems involving linear boundary motion, the layering scheme is often sufficient.
• For example, flow around a check valve can be simulated using only the layering scheme.
• Another example of dynamic meshing can be while simulating the CFD of a fan.
• In this case, the fan has a rotational motion, and the user defined function is defined accordingly.
• Examples –
• Turbine fan
•  
• Fluid sloshing in gearbox simulation
•  
• CFD Analysis of Needle Free Liquid Jet InjectorsCFD Analysis of a 

• Diaphragm-less Shock Tube

 What is the fluid Sloshing effect? Discuss whether the sloshing effect is good or bad? Explain. 

 

• Fluid sloshing refers to the movement of liquid inside another object (which is, typically, also undergoing motion).
• Strictly speaking, the liquid must have a free surface to constitute a slosh dynamics problem, where the dynamics of the liquid can interact with the container to alter the system dynamics significantly. 
• Important examples include propellent slosh in spacecrafts, tanks and rockets (especially upper stages), and the free surface effect (cargo slosh) in ships and trucks transporting liquids (for example oil and gasoline).
• Such motion is characterized by "inertial waves" and can be an important effect in spinning spacecraft dynamics.
• Extensive mathematical and empirical relationships have been derived to describe liquid slosh.
• These types of analyses are typically undertaken using computational fluid dynamics and finite element methods to solve the fluid structure interaction problem, especially if the solid container is flexible.
• Relevant fluid dynamics non-dimensional parameters include the bond number, the Webber number, and the Reynolds number.
• In essence, fluid sloshing effect is good in some cases, and bad in other cases. It basically depends on the situation or problem statement.
• In this particular case, fluid sloshing is beneficial to allow proper and uniform lubrication of all the teeth.

 

What is the use of UDF? 

 

• User-defined functions allow programmers to create their own routines and procedures that the computer can follow.
• It is the basic building block of any program and also very important for modularity and code reuse since a programmer could create a user-defined function which does a specific process and simply call it every time it is needed.
• A user-defined function, or UDF, is a function that you program that can be dynamically loaded with the Ansys fluent solver to enhance the standard features of the code. For example, you can use a UDF to define your own boundary conditions,material properties, and source terms for your flow regime, as well as specify customized model parameters (e.g., DPM, multiphase models), initialize a solution, or enhance postprocessing.
• UDFs are written in the C programming language using any text editor and the source code file is saved with a .c

 

 Discuss the common errors that occurred in the simulation. A] 'Dynamic mesh failed' error. B] 'Negative cell volume detected' error.

• The dynamic mesh failed error and negative cell volume detected error are the most common issues faced while running simulations with dynamic meshes.
• The first reason, one of these issues may arise is due to a bad mesh quality.
• Both for the unstructured and structured mesh types, if the quality of majority of the cells is not high, it may result in computation errors thus causing the simulation residuals to crash.
• Also, it is advisable to check the volume of the smallest mesh cell.
• A very small motion of the boundary can lead to the collapse of the cell thus leading to this particular error.
• Another factor is to make sure that all the boundaries of each gear are selected and not a single curve is left out.
• In this case, if we fail to select even a small curve, then that particular curve will be stationary and the other boundaries will collapse into it thus resulting in a negative cell volume error.
• Also, the time step size should be considerably small to allow each and every movement to be captured.
• A high time step size may result in this error