Gearbox Sloshing effect using Ansys Fluent
Introduction :
In this project we perform a gearbox sloshing effect using ansys fluent for 2 two different clearances of same spur gears with 2 different fluids. In fluid dynamics slosh refers to the movement of liquid inside another object which is also undergoing certain motion.
(Gearbox)
This study is done in the Gear design & manufacturing industry on gearboxes & even individual or paired gear pairs of different types to study the fluid - gear teeth contact behaviour. Understanding Lubricants behaviour, Transmission fluid etc.
Sloshing effect has other research purposes as well coupled with dynamic meshing & sliding meshes in ansys fluent for example in study of compressor fluid behaviour.
Gear Pair :
The gear Box is designed and imported in Ansys.
Objective :
1. Dynamic Meshing - Add function for Motion of left & right Gear pair.
2. Analyze the flow patter of fluid for two different clearances of the spur gear geometry
3. Analyze the flow with 2 different fluids - 1. Water , 2. Oil.
Geometry Preparation in SpaceClaim :
The Gearbox geometry as you see above in 3D is converted into 2D to save computational Time and considering the Limits of meshing & Computational power available.
Firstly the Fluid Volume is extracted using edge selection method.
Then geometry is Split using Split body Command from the plane and then half section is removed.
The Orange section is then selected and Copy - pasted into New design to Create the 2D geometry.
The 2D section Obtained in the New design looks as shown below. The older design is then simply closed as its not needed anymore and this new 2D design is imported in the Ansys fluent.
This Gearbox has Lesser Clearance or Tight clearance. Gearbox with Higher clearance between gear pairs is also prepared similarly.
Meshing :
Less Clearance :
This is the Geometry with less clearance, The mesh created is of 2mm with 17078 element size and 10004 Nodes.
Higher Clearance :
This is the geometry with Higher clearance, The mesh created is of 2mm with 17429 element size and 10226 Nodes.
User Defined Functions : Ansys Fluent :
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]*/
}
Flow time calculation to determine Time step size and No. of Time steps in ansys fluent :
As aforementioned the angular velocity is determined to be 200 rad/s. 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 Computational time & capacity 2 rotation is selected for this project.
`omega = (2*pi*N)/60` , 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 for 1 Rotation the seconds we require is :
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.
With this calculated we move to case set up .
Case Set up :
Set up 1 for Less & Higher clearance model using Water as Fluid.
Solved using Serial Procesor.
1. Solver : Pressure Based.
2. Velocity Formulation : Absolute
3. Time : Transient Case
4. 2D space : Planar
5. Gravity enabled -y dir.
6. Viscous Model : K-eps 2 eqn ( std)
7. Multiphase : Vof : Implicit : 2 eulerian phases.
Primary Phase : Air
Secondary Phase : Water ; Density : 998.2 Kg/m^3 ; Viscosity : 0.001003 kg/m-s.
8. Dynamic Mesh :
Smoothing enabled - Diffusion
Remeshing enabled : Local cell, Local Face .
Min Length Scale (m) : 0
Max Length Scale (m) : 0.0033
Max Cell Skewness : 0.4
Max face Skewness : 0.4
Size remeshing Interval : 2
9 . Dynamic Mesh zones Rigid body for Left & right gear from the UDF file based on CG of the Gear pair left and right respectively (location wise)
10. Solution : Simple scheme : first order ; Hybrid Initialization
11. Patching Phase 2 (water) : Volume fraction with Created region (shown after case set up)
Set up 2 for Less & Higher clearance model using Oil as Fluid.
Everything is exactly same as Set up 1 except for the following :
1. Secondary Phase : Oil ; Density : 871 Kg/m^3 ; Viscosity : 0.04006889 kg/m-s.
2. Patching Phase 2 (Oil) : Volume fraction with Created region (shown after case set up)
Region Creation :
Under Adapt settings, there is a region option, where we specify a Quad shaped region for our geometry, This region is where the Fluid will initially be held at 0 Iteration/ flow time and iterate from here. Patching of volume fraction is done with this region.
For Less clearance Model - Region :
(meters)
Xmin : -0.05612 Xmax : 0.17112
Ymin : -0.0675 Ymax : -0.0375
For High clearance Model - Region :
(meters)
Xmin : -0.15 Xmax : 0.175
Ymin : -0.0675 Ymax : -0.0375
Solution and Post Processing :
1. Less Clearance Model with Water as Fluid :
Residual : The Equations converge at about 24000 iterations and thereby vary in steps.
Animation :
2. Less Clearance Model with Oil as Fluid :
Residual : The Equations converge at about 11000 iterations and thereby vary in steps.
Animation :
3. High Clearance Model with water as Fluid :
Residual : The Equations converge at about 11000 iterations and thereby vary in steps.
Animation :
4. High Clearance Model with Oil as Fluid :
Residual : The Equations converge at about 11000 iterations and thereby vary in steps.
Animation :
Results and Conclusions :
1. Sloshing effect is observed in both Less and higher clearance model.
2. Oil being Lighter but with higher viscosity than water has tendency to cling to the surface in the teeth tighter than the water during rotation.
3. Being viscous oil also slides slower than water from the walls sides in the fluid volume.
4. The sloshing effect is more in the Less clearance model as the fluid is compressed to flow in small volume space. While fluid smoothly moves through high clearance model still creating a smaller backlash slosh .
5. Higher Meshing along with more rotations are required to observe the fluids in depth effects on the model.
References :
1. Udf Manual : https://www.afs.enea.it/project/neptunius/docs/fluent/html/udf/main_pre.htm
2. https://www.microsoft.com/en-in/download/details.aspx?id=44266
----------------------------------------------- THE END ------------------------------------------------