Gearbox Sloshing simulation using Ansys Fluent

Objective: To analyzed the flow pattern of fluid inside gearbox using various configurations.

Cases to be considered:
1. 20% immersion, Fluid- Engine oil
2. 30% immersion, Fluid- Engine oil
3. 20% immersion, Fluid- n-heptane liquid
2. 30% immersion, Fluid- n-heptane liquid

Given: CAD file to import into Spaceclaim. and script file to define UDF to give motion to boundaries.

Theory:

                                                  `tt"Gearbox Lubrication"`
Gears are toothed, mechanical transmission elements used to transfer motion and power between machine components. Depending on the design and construction of the gear pair, the transference of motion between the driving shaft and the driven shaft can result in a change in the direction of rotation or movement.
Additionally, if the gears are not of equal sizes, the machine or system experiences a mechanical advantage which allows for a change in the output speed and torque (i.e., the force which causes an object to rotate).
Due to its extensive operation, it is required to provide proper lubrication.
The purpose of lubricating gears is as follows:
1. To reduce the friction between two parts.
2. To reduce the wear of moving parts.
3. To act as a cooling medium.
4. To keep engine parts clean.
5. To absorb shock between bearings and other parts.
6. To prevent deposition of carbon and metallic components from corrosive attacks.
7. To resist oxidation.

There are three methods of lubrication:
1. Grease lubrication.
2. Splash lubrication (oil bath method).
3. Forced oil circulation lubrication.

Grease lubrication is suitable for any gear system that is open or enclosed. It is suitable for low-speed operation, but it provides less cooling than oil and is not recommended for continuous-duty or heavily loaded applications, even at low speeds.

Oil splash lubrication is often used for helical, spur, and bevel gearboxes. It is used with enclosed. The rotating gears splash lubricant onto the gear system and bearings. It needs at least 3m/s tangential speed to be effective. However, splash lubrication has several problems but two of them are oil level and temperature limitations.
Oil level- There will be excess agitation loss if the oil level is too high. On the other hand, there will not be effective lubrication or the ability to cool the gears if the level is too low.
Temperature- The temperature of a gear system may rise because of friction loss due to gears, bearings and lubricant agitation which causes Lower viscosity of the lubricant, Accelerated degradation of lubricant, Deformation of housing, gears, and shafts and decrease backlash.

Forced lubrication applies lubricant to the contact portion of the teeth by means of an oil pump. There are drop, spray, and oil mist methods of application.
Drop Method- An oil pump is used to suck-up the lubricant and then directly drop it on the contact portion of the gears via a delivery pipe.
Spray Method- An oil pump is used to spray the lubricant directly on the contact area of the gears.
Oil Mist Method- Lubricant is mixed with compressed air to form an oil mist that is sprayed against the contact region of the gears. It is especially suitable for high-speed gearing.
Oil tank, pump, filter, piping and other devices are needed in the forced oil lubrication system. Therefore, it is used only for special high-speed or large gearbox applications.

`tt"CASE SETUP"`

STEP-1: Import the geometry into SpaceClaim.

STEP-2: Extract Fluid volume.

STEP-3: Create 2D geometry using the Split body.
After splitting the body into two half, the face of the fluid domain selected, copied and pasted into a new design.
Delete rest of the geometry files.

STEP-4: Meshing.

The complete domain has been discredited with a mesh element size of 30mm.
Since we are interested in simulating 2D geometry, the completed mesh element changed to Triangular mesh.
Capture Proximity- Yes
Nos of cells across gap- 1

Naming: 

`tt"FLUENT SETUP"`

Viscous Model- Realizable k-epsilon with Enhanced near-wall treatment.

Multiphase-
Volume of fluid (VOF) with Two eulerian phases.
Implicit Formulation

Materials-
Air, Engine oil and n-heptane liquid choose according to the case we want to simulate

Phases-
Phase 1- Air
Phase 2- Engine Oil OR n-heptane

Adapt-
As we are simulating the two cases i.e. 20% and 30% immersion. This means 20% or 30% of complete geometry filled with lubricant. Then in order to set or adapt the region which will define immersion we need to register cells accordingly.

For 20% immersion:

X_max= 0.1689,   X_min= -0.05383
Y_max= -0.04081, Y_min= -0.08818

For 30% immersion:

X_max= 0.17686, X_min= -0.06186
Y_max= -0.027,    Y_min= -0.085

Dynamic Mesh- This model helps us to simulate the model flows where the shape of the domain is changing with respect to time due to motion on the domain boundaries.
In this case, the motion of gear is defined by User-defined Function (UDF) where gears are rotating with an angular velocity of 200 rad/sec.

Mesh Method setting:
Smoothing- Diffusion
Layering- Height based
Remeshing- Go with default values
Minimum length scale- 4.79e-6
Maximum length scale- 0.010389
Maximum cell skewness- 0.5

A complete domain is Initialized with Hybrid Initialization method.

`tt"SOLUTION"`

Time calculation:

`tt"Angular Velocity of gear= 200 rad/sec"`

`tt"RPM of gear will be calculated as"`:
`omega=(2*pi*N)/60`

`tt"RPM= 1910.82"`
`tt"RPS= 31.847"`

`tt"Total time required to complete one revolution will be"`

`tt"Time per revolution= 0.0314 sec"`

CASE-1: 20% immersion, Fluid- Engine oil.

20% of the Fluid domain is filled with engine oil for lubrication.

Residual plots:

The below image shows how the lubrication of gear is being done until the second rotation of the gear.

Animation:

CASE-2: 30% immersion, Fluid- Engine oil.

30% of the Fluid domain is filled with engine oil for lubrication.

Residual plots:

Lubrication in gear at different time intervales.

Animation:

CASE-3: 20% immersion, Fluid- n-heptane liquid

20% of the Fluid domain is filled with n-heptane for lubrication.

Residual plots:

Lubrication in gear at different time intervals.

Animation:

CASE-4: 30% immersion, Fluid- n-heptane liquid

30% of the Fluid domain is filled with n-heptane for lubrication.

This simulation we were able to run for little fewer nos. of iterations than the rest of the cases due to limitations imposed by the academic license of fluent.

Residual plots:

Lubrication in gear at different time intervales.

Animation:

`tt"Observation:"`

In this study, we have simulated gear lubrication with various configurations one with two different immersion values 20% and 30% and another one with two different fluids of different viscosity i.e. Engine oil and n-heptane.

Here, our study is limited only for 2 rotations i.e. 0.068 sec of gear because of working constraints of the academic license of Ansys Fluent

`***`At time t= 0 sec, all lubricating oil is concentrated at the bottom and sidewalls of a gearbox, 30% immersion configuration has more lubricant than that of 20% immersion configuration.

`***` As gear starts rotating 30% immersion configuration has enough lubrication to the filled gap between teeth, right from first rotation of the gear. On the other hand, 20% immersion configuration, the gears are in a loss‐of‐lubrication operating condition for a long time, their heat dissipation performance would deteriorate, and thus result in a drastic increase in tooth temperature, even scuffing failure.

`***`Splashing of lubricant helps to spread the lubricant on all over parts in both immersion configurations but 30% immersion configuration is more effective.

`***` Engine oil (mu= 1.06 kg/ms) is more viscous than n-heptane (mu= 0.000409 kg/ms), hence it has more benefits over another while operating at higher temperature as it increases in viscosity results in lower oil consumption and less wear, which is profitable for the environment.

`***`Engine oil has more ability to stick to the tooth surface due to high viscosity resulting in appropriate temperature distribution.

Dynamic meshing: It is a meshing technique or Ansys fluent capability used to simulate problems with boundary motion, such as check valves and store separations.
More precisely saying, the Dynamic meshing model is used to model the flows where the shape of the domain is changing with time due to motion on the domain boundaries. Motion can be anything translational, rotational.

Dynamic meshing is used with both steady and transient state applications. For steady-state application, we can use dynamic meshing where it is beneficial to move the mesh in the steady-state solver.
Motion can be prescribed or unprescribed. Prescribed motion is that where you can specify linear and angular velocity about CG of a solid body with time. Unprescribed motion is where the motion of a solid body is determined based on the solution of the current time.

Different mesh motions schemes may be used for different zones. Connectivity between adjacent zones may be non-conformal.

1. Spring analogy (Spring smoothing)- The nodes move as if they are connected via springs, or as if they were part of the sponge. Connectivity remains unchanged. This scheme is limited to relatively small deformations when used as a stand-alone meshing scheme. Available for tri and tet meshes, May be used with quad, hex and wedge mesh element types, but that requires a special command.

2. Local Remeshing- As user-specified skewness and size limits are exceeded, local nodes and cells are added or deleted. As cells are added or deleted connectivity changes. Available for tri and tet meshes.

3. Layering- Cells are added or deleted as the zones grow or shrinks. As cells are added or deleted, connectivity changes. Available for quad, hex and wedge mesh elements.

Examples- Automotive piston moving, A flap moving on an airplane wing, an artery expanding and contracting, gearbox, etc.

Advantages- Boundaries/Objects motion can be moved based on In-cylinder motion (RPM, stroke length, crank angle, …), Prescribed motion via profiles or UDF, Coupled motion based on hydrodynamic forces from the flow solution, via FLUENT’s 6 DOF model.

Sloshing: Sloshing means any movement of the free liquid surface inside its container. It is caused by any disturbance to partially filled liquid containers. In particular, liquid sloshing on the free surface may have a significant influence on the response of the container. 

Sloshing is also a periodic motion of the free surface of the liquid in a partially filled tank or container that can be caused by several factors. It is viewed in many applications.
In freely slosh it can produce forces that cause instability, rollover, and failure or damage in tank or container in some cases.
Baffles used as sloshing suppression devices.

The severity of sloshing and its dynamic pressure loads depend on the tank geometry, the depth of the liquid, the amplitude and the nature of the tank motions. They also depend on the frequency of excitation over a range of frequencies close to the natural frequency of the fluid.

Sloshing of liquid in the storage tank may result in negative effects such as deformation and failure of tank walls due to impact. If an open tank is subjected to ground motions, sloshing may lead to liquid spillage. Therefore, sufficient clearance needs to provide between the free surface and top of the tank or roof must be provided.

User-Defined Function (UDF): It is a C program or C function that can dynamically be loaded into Ansys Fluent to enhance the standard features or its capabilities.
For example, we can use a UDF to define our own programmed 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 extension (e.g., myudf.c). One source file can contain a single UDF or multiple UDFs, and you can define multiple source files.

UDFs are defined using DEFINE macros provided by ANSYS FLUENT. They are coded using additional macros and functions also supplied by ANSYS FLUENT that access ANSYS FLUENT solver data and perform other tasks.

Every UDF must contain the udf.h file inclusion directive ( #include "udf.h") at the beginning of the source code file, which allows definitions of DEFINE macros and other ANSYS FLUENT-provided macros and functions to be included during the compilation process.
Note that values that are passed to a solver by a UDF or returned by the solver to a UDF are specified in SI units.

Source files containing UDFs can be either interpreted or compiled in ANSYS FLUENT.
For interpreted UDFs, source files are interpreted and loaded directly at runtime, in a single-step process.
For compiled UDFs, the process involves two separate steps. A shared object code library is first built and then it is loaded into ANSYS FLUENT. 
After being interpreted or compiled, UDFs will become visible and selectable in ANSYS FLUENT dialog boxes and can be hooked to a solver by choosing the function name in the appropriate dialog box.
In summary, UDFs:
`***`are written in the C programming language.
`***`must have an include statement for the udf.h file.
`***`must be defined using DEFINE macros supplied by ANSYS FLUENT.
`***`utilize predefined macros and functions supplied by ANSYS FLUENT to access ANSYS FLUENT solver data and perform other tasks.
`***`are executed as interpreted or compiled functions.
`***`are hooked to an ANSYS FLUENT solver using a graphical user interface dialog box.
`***`use and return values specified in SI units.

The source file of UDF we use in this case to give motion to the boundary.

#include "udf.h"

DEFINE_CG_MOTION(right_motion, dt, vel, omega, time, dtime)
{
	vel[0] = 0.0;
	vel[1] = 0.0;
	vel[2] = 0.0;

	omega[0] = 0.0;
	omega[1] = 0.0;
	omega[2] = 2.0e2; /* [rad/s]*/
}
DEFINE_CG_MOTION(left_motion, dt, vel, omega, time, dtime)
{
	vel[0] = 0.0;
	vel[1] = 0.0;
	vel[2] = 0.0;

	omega[0] = 0.0;
	omega[1] = 0.0;
	omega[2] = -2.0e2; /* [rad/s]*/
}