SIMULATION ON SLOSHING OF GEAR BOX
Gearbox Sloshing effect
OBJECTIVE :
- To perform gear sloshing simulation using Ansys fluent for two different gearboxes with different clearance.
- To understand and implement the Dynamic Meshing option ad optimise it for accurate result.
- To use the UDF – User defined function option to define the motion of the gears in pair.
- To compare the 4 cases with different immersions and materials
Fluid-Engine Oil
1.20% Immersion-Fluid .
2.30% Immersion-Fluid .
Fluid-n-heptane (c7h16)
3.20% Immersion-Fluid .
4.30% Immersion-Fluid .
SOFTWARE USED:
ANSYS, SpaceClaim - To prepare FV model.
ANSYS, Meshing - To mesh the given model.
ANSYS, FLUNET - To setup the boundary conditions and to solve the given model.
ANSYS, CFD Post - To perform Post Processing.
THEORY :
What is Dynamic meshing? Give some other examples where dynamic meshing can be used
The dynamic mesh model allows you to move the boundaries of a cell zone relative to other boundaries of the zone, and to adjust the mesh accordingly. The boundaries can move rigidly with respect to each other (that is, linear or rotational motion), and/or deform.
Dynamic Mesh Model is a method by which the solver(FLUENT) can be instructed to move boundaries and/or objects and to adjust the mesh accordingly.
Examples :
- Automotive piston moving inside a cylinder.
- A flap moving on an airplane wing.
- A valve opening and closing .
- An artery expanding and contracting.
For information indetail Click on the link : Click Here
What is the fluid Sloshing effect? Discuss whether the sloshing effect is good or bad?
In fluid dynamics, slosh refers to the movement of liquid inside another object (which is, typically, also undergoing motion).
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 propellant slosh in spacecraft tanks and rockets (especially upper stages), and the free surface effect (cargo slosh) in ships and trucks transporting liquids (for example oil and gasoline). However, it has become common to refer to liquid motion in a completely filled tank, i.e. without a free surface, as "fuel slosh".
A) Dynamic mesh Failed error :
Apply under-relaxation
Under-relaxation is a simple yet effective technique for updating the fields between iterations. The default way to update the field values in a new iteration would be to simply ignore the old value and replace it with the new values.The standard way to deal with this is under-relaxation and is very effective. Instead of replacing the field values with the new result, it is better to update with a weighted average between the old and the new values.
Typically, we suggest starting with
- 0.7 for velocity
- 0.3 for pressure and other scalar fields
If the simulation diverges, try using lower relaxation factors (say 0.3 for velocity and 0.1 for pressure).
You can find this values under the Step3: setup ----> solution controls . As you go down in this page.
Solvers
- Use coupled implicit solver if possible.
- You can choose the GAMG and smooth solver. Especially smoothSolver performs quite well when the matrices have bad conditions.
Processor
- Running in series or parallel with a single processor sometimes helps.
For more information Click on the Link : Click Here
B) Negative cell volume detected error :
- Check all mesh quality parameters and maintain the skewness(skewness under 0.8), aspect ratio within the appropriate range.
- The bad mesh can lead to floating-point errors. Try to use conformal mesh because interfaces are prone to give this error.
You find the values those I have used in this Simulation under the Step3: setup ----> Meshin methods controls . As you go down in this page.
For more information Click on Link : Click on this Link
PROCEDURE :
STEP 1 : GEOMETRY
1.Importing the 3D model:
The first step is to import the 3D model to the space claim.
3-D View Sectional View
Lubricant Flow Region left and right Gears
2.Volume extraction:
Fluid volume extraction is defined as extracting the volume of the fluid .
In this case,we are extracting the volume of the fluid region.Here,the space occuied by the gear and lubricant is the fluid medium.
3.Extracting the 2D model:
- The next step is to extract the 2D model from the 3D geometry
- The 2D model is extracted by creating the planes along the three axis and splitting the body of the 3D model by suing the split body tool.
- After that the splitted body is copied and pasted into the another geometry.
STEP 2 : MESHING
Physics Preferences : CFD Capture Proximity : Yes
Solver preferences : Fluent Proximity min Size : 0.3 mm
Element Order : Linear Num Cells Across Gap : 1
Element size : 2 mm
Method : Triangles
Statistics :
Nodes = 10420
Elements = 17754
STEP 3 : SET UP & SOLUTION
- Solver type: pressure based
- Time state: Transient
- Enable gravity with -9.81m/s on y-axis
- Viscous Model : Viscous-K epsilon-"Realizable"-'Enhanced wall function'
- Uncheck the energy since we don’t deal with temperature.
- model: Multiphase model with Volume of fluid method
- Formulation method: implicit
- No boundary conditions
- Materials used:
- Air + Engine OIL for case 1 & 2
- Air + n-heptane_liq for case 3 & 4
**Engine Oil Properties:- Density= 889 kg/m3, Dynamic Viscosity = 1.06 kg/m-s**
**n-heptane Properties:- Density= 684 kg/m3, Dynamic Viscosity = 0.000409 kg/m-s**
** Air Properties:- Density= 1.225 kg/m3, Dynamic Viscosity = 1.7894e-05 kg/m-s**
User Defined Functions (UDF) :
This is a udf file known as user defined function, it can be added in Ansys fluent functions to give motions or define certain terms, custom boundary conditions, material properties, source term wrt to the simulation being performed. It is used in ansys fluent solver to enhance the standard features of the code.
This udf function is determining the angular velocity omega in Z direction of the right and left gear pairs as 200 rad/s in opposite direction respectively. ( The gear pairs in 2D geometry are in XY plane) .
#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]*/
}Initialization: Standard **
Patch: phase - water
variable- volume fraction
heavier fluid value as 1 and lighter fluid as 0
*patching should be done individually for different fluids and should be done every time after initialization
*Also , Mark/Adapt to be done for every time after intialization.
20% Immersion fluid region :
30% Immerson Fluid region :
Use appropriate time step based the case as follows :
**NOTE** :
- As above mentioned the angular velocity is taken as 200 rad/sec
- we need to calculate the flow time for 1 rotation of the gear pair to set up the time step size and No. of time steps accordingly to achieve 2 rotations minimum.
- In industry standard practice is usually about 5-6 rotations but considering about the adcemic license & Computational time , we proceeded with 2 rotation for this project.
Flow time calculation to determine Time step size and No. of Time steps in ansys fluent :
, where Omega : 200 rad/s
Therefore, N = 1909 Rpm .
N/60 = 1909/60 = 31.83 Rps.
This means we get 31.83 rotations per second.
So , how many seconds does it takes for 1 Rotation :
1/31.83 = 0.0314 seconds of flow time.
So for 2 Rotations we need,
2/31.83 = 0.0628 seconds of flow time.**
Determining Time step size and No. of time steps for all cases :
" Time step size * No. of Time steps = Total flow time."
we know the flow time as 0.0628 seconds,
Therefore by choosing Time step size as 0.0001, we get No of Time steps as:
No of Time steps = 0.0628/0.0001 = 628.
For the Simulation the choosen Time step is 650 which will give results just slightly over 2 rotations for all cases.
Finally , Time step size = 0.0001
No. of time steps = 650
Meshing methods Solution_methods solution_Controls
STEP 4 : RESULTS
Overview :
STEP 4 : RESULTS
CASE 1 : Engine oil + Air ; 30% Immersion region
Residuals :
Animation Vedio :
CASE 2 : Engine oil + Air ; 20% Immersion region
Residuals :
Animation Vedio :
CASE 3 : n-heptane + Air ; 30% Immersion region
Residuals :
Animation Vedio :
CASE 4 : n-heptane + Air ; 20% Immersion region
Residuals :
Animation Vedio :
Conclusion :
- It is observed that the formation of engine oil lubricant film over a gear tooth is more stable than n-heptane as a lubricant on it.
- Sloshing effect is more in the lubricant which will have lower viscosity.
- In this simulation , we can say that Viscosity of n-heptane( 0.000409 kg/m-s) << Viscosity of engine oil(1.06 kg/m-s) .
- As we observed in the case 1 & 3 , n-heptane sloshed everywhere unlike the engine oil .This is because n-heptane has less viscosity when compared with engine oil.
REFERENCES :
Theory of Dynamic Meshing for Gearbox Sloshing problem. : Skill Lync
https://en.wikipedia.org/wiki/Slosh_dynamics