Simulation of sloshing of Fluids inside Gear box using Ansys Fluent

Abstract:

The following report discusses in detail the phenomenon of sloshing of fluids inside a gear box. Complete modelling of the  problem from geometry preparation, to meshing, multiphase modelling is set up. The effects of two fluids , engine oil and n-heptane liquid is studied on 20% and 30% of the volume.  Animation files and their links to acess is provided with the report. 

Key words- Fluent, Dynamic meshing, user defined function, multiphase modelling, Volume of fluid 

Introduction:

Sloshing of fluids:

In fluid dynamics slosh refers to the movement of fluid inside an object. The liquid mus have a free surface to constitute the slosh dynamics problem. The liquid can interact with the container to modfy the dynamics . Examples of slosh dynamics include slosh of propellant in aircraft tanks and and space craft dynamics. The dimensionless numbers that are involved include Reynolds number, Bond number.

Slosh was a factor in Falcon 1 second test flight anamoly and has been implicated in various other flight anamolies including a near disaster with near Earth Rendzevous eart satellite. 

Use of user defined function (UDF):

An user defined function (UDF) is a function that can be dynamically loaded with Ansys fluent solver to enhance the standard features of the code. Its uses are :

• To define own boundary conditions
• to define material properties
• To specify source terms of flow regime
• To specify customized model parameters like in discrete phase modeliing and multi phase modelling 
• To initialise a solution
• To enhance postprocessing

A shared object code library is first built in Ansys fluent then it is loaded.

To summarize:

• UDF is written in C language 
• must have include statement for the udf.h file
• must be defined using the DEFINE macros supplied by fluent
• executed as interpreted or compiled. In this analysis, it is executed as compiled
• use and return values secified in SI units

Dynamic meshing:

The dynamic mesh model can be used to model flows where the shape of the domain is changing with time due to motion on the domain boundaries. the motion can be prescribed motion (where the angular velocity or the rotational motion i s provided) or the unprescribed motion. The following analysis is an prescribed motion. The unprescribed motion is handled by the six degree of freedom solver that ansys fluent provides. Ansys Fluent aloows to provide the  motion either by boundary profiles, user defined function or six degree of freedom solver. Fluent expects the motion to be described either on cell zone or faces. If the model contains moving and non-moving regions, it is needed to identify these regions by grouping them into their respective face or cell zones in the starting volume mesh that is generated. Furthermore, regions that are deforming due to motion on their adjacent regions must also be grouped into separate zones in the starting volume mesh. The boundary between the various regions need not be conformal. 

• Dynamic mesh update methods:

There are three ways to update the dynamic mesh :

1) Smoothing 

2) Dynamic layering

3) Local remeshing methods

Further more there are three types of smoothing methods :

1) Spring based smoothing methods- In the spring-based smoothing method, the edges between any two mesh nodes are idealized as a network of interconnected springs.

2) Laplacian smoothing methods- Laplacian smoothing is the most commonly used and the simplest mesh smoothing method. This method adjusts the location of each mesh vertex to the geometric center of its neighboring vertices. This method is computationally inexpensive but it does not guarantee an improvement on mesh quality, since repositioning a vertex by Laplacian smoothing can result in poor quality elements.

3) Boundary layer smoothing method- The boundary layer smoothing method is used to deform the boundary layer during a moving-deforming mesh simulation. For cases that have a Mesh Motion UDF  applied to a face zone with adjacent boundary layers, the boundary layer will deform according to the UDF that is applied to the face zone. This smoothing method preserves the height of each boundary layer and can be applied to boundary layer zones of all mesh types (wedges and hexahedra in 3D, quadrilaterals in 2D).

• Remeshing methods:

On zones with triangular mesh, spring based smoothing method is generally used. When the boundary displacement is large compared to the local cell sizes, the cell quality can deteriorate or the cells can become degenerate. This will invalidate the mesh (e.g., result in negative cell volumes) and consequently, will lead to convergence problems when the solution is updated to the next time step. 

To solve this [roblem, Ansys fluent, agglomerates cells that violates skewness or the size criteria and locally remeshes the agglomerated cells or faces. If the new cells , satisfy the skewness criterion, they are updated, else discarded.

Various remeshing methods included in ansys fluent are:

• Local remeshing
• Local face remeshing
• Face region remeshing
• 2.5D remeshing 

Among the four options, local face remeshing and the 2.5D remeshing are for 3D flows. In our analysis as it is 2D Geometry, local remeshing is done.

since my analysis demands only local remeshing, The local remeshing technique is described in details:

Using the local remeshing method, ANSYS FLUENT marks cells based on cell skewness and minimum and maximum length scales as well as an optional sizing function.

Ansys fluent evaluates each cell and marks it for remeshing if it meets one or more of the following criteria:

 

• It has a skewness that is greater than a specified maximum skewness.
• It is smaller than a specified minimum length scale. 
• It is larger than a specified maximum length scale.
• Its height does not meet the specified length scale (at moving face zones, e.g., above a moving piston)

 The different type of errors faced in the analysis is discussed at the end of the report.

The following part deals with the modelling of the problem and simulation set up.

Geometry:

A gear train step file is imported into space claim. The olume is extractedusing the edge select tool. The region of interest is selected and a new design is openned. Chosing the xy plane the same is pasted. The 3D geometry is transformed into 2D geometry

  

Mesh:

Once the 2D modified geometry is imported to the ansys mesh. The geometry basically has two components, the left gear and the right gear. 

The global mesh control of Ansys is used to make global adjustment in the meshing strategy that includes sizing functions, inflation,smoothing ,defeaturing,etc etc. Under the Mesh, ther is defaults and in that lies the Physics prefernce. Out of the four available options, CFD is selected And in thet Fluent is ticked. Mesh settings defaults are automatically selected to meet the Physics preference and the solver needs.

Element size is provided that essentially is used for meshing the all edges ,faces and bodies. 

Under sizing, There is advanced sizing function(ASF). The proximity is turned on. Proximity controls the mesh resolution in the proximity regions of the model. This fits in specified number of elemnts in the narrow gaps. The higher the number of cells across the gaps, creates more refined mesh. 

By looking at the statistics , the nuber of elements and cells can be watched for. Since it is academic license, there is abar upto which the number of cells can be varied to.

Element size	0.001(meters)
Nodes	15904
Elements	28361

Mesh quality:

Mesh quality needs to be maitained because;

• Good mesh quality means criteria re within the given range
• Solution is grid independent
• Mesh is valid for the studied physics.

Mesh metrices:

1) Orthogonal quality:

minimum	6.86e-002
maximum	1
average	0.96194
standard deviation	4.19e-002

 

The minimum is 0.88, so it falls under the very good catagory. Low orthogonal quality values are not wanted.

2) Skewness:

Minimum	1.6463e-007
Maximum	0.95702
Average	6.204e-002
Standard deviation	6.723e-002

 

The maximum skewness is between 0.25 and 0.38. So it can be considered as a very good. In general , maximum skewness should be ess than 0.95. High skewness values are not wanted.

Named selection:

There are two named selections, Right gear and left gear. This Analysis donot have any boundary conditions but the named selection is done for applying the dynamic meshing. Care is taken so that all the edges are selected for both the gears using a Edge select tool. There are approx 299 edges in both the gears respectively.

     

 

Solving and Fluent Set up:

The meshed model is transported to the fluent set up for stting up of physics and other solver requirements.  The flow chart is as follows 

• Specifying general conditions
• Domain controls(mark and adpt cells, Dynamic meshing)
• Modelling ( Viscous, Multiphase)
• Loading and adding UDF
• Initialisation, patching, Solve 
• Examine animation of the contour plots

 1) General conditions:

Transient solution is looked for. The gravity is turned on. As the 2D image is in x-y plane, the accelaration due to gravity is set to -9.81m/s^2 along the y plane. Pressure based solver is used. The ambient pressure is 1ATM. Temperature donot play a role here.

   

2) Domain control:

This study involves 4 cases with two different fluids and two different percentages. Here the cells are marked for all the cases. 20% and 30%. The total height of the 2D gear box is 135 mm . 20% and 30% of that height is hand calculated and corresponding co-ordinates are found out. The cells are marked by clicking the cell register- new -region. The xminimum,xmaximum,yminimum,ymaximum values are put in.

The above image is for 30% engine oil. The region created is important while patching .

Dynamic meshing: The dynamic meshing is important when a solid object in flow domain is moved with a prescribed motion or under hydrodynamic forces. Two motions are created for the left and right gear by clicking the create /edit tab. The center of rotation of the left gear is (0,0,0) and for the right gear is (0.115,0,0). All these are rigid body motions. 

There are three possible ways of dynamic mesh update :

Layering, smoothing and Remeshing. 

The remeshing parameters are :

    

Minimum length scale	1e-5
Maximum length scale	0.001
Maximum cell skewness	0.7
Size remeshing interval	5

• The complied user defined function is loaded from the machine. The library is builtand the UDF is loaded. The UDF has the rotational otion for the gear.

Modelling:

Viscous modelling:

The turbulence modelling for this analysis is chosen and  realizable K-epsilon and enhanced wall treatment. The energy is turned off, since temperature donot play a role here.

 

 

Multiphase modelling:

VOF method:

The Volume of fluid methods available with Fluent uses a pressure based solver. It is not available with the density based solver. The total control volume/volumes should be filled with single or multiphase fluidas the VOF method donot allow voids.

This uses transient solutions, since this problem donot have distinct inflow boundaries. The VOF relies on the fact that the two fluids are not interpenetrating.For each phase added, a variable is introduced called the volume fraction of the phase in computational cells.In each case the summation of the volume fraction of all phases sums to unity.

The tracking of the interphase between the phases is accomplished by solution of a continiuty equation for volume fraction of one or more phases .

`(1/rho(q))*[(del)/(del(t))*(alpha(q)*rho(q)+nabla.(alpha(q)*rho(q)*v(q))]=S(alpha.e)+summation(m(pq)-m(qp))`----(1)

In the above equation , 

`m(pq)`= mass transfer from p phase to q phase

`m(qp)`= mass transfer from q phase to p phase

`S(alpha.e)`= mass source for each phase and is 0.

The volume fraction equation wont be solved for the prmary phase, for the primary phase the volume fraction equation is :

`summation(alpha(q))=1`---(2)

   

 

 

The case is initialized and held for patch generation

In patch , the register to patch is the region created during mark and adapt cells, The method is VOF, and the phase 2 is patched to value 1. The phase 2 or secondary phase is the engine oil and the n-heptane liquid in terms. 

Contours are created to check the volume fraction of secondary phase. an animation is also created to see the simulation. 

 

The above image is the contours of secondary phase wih volume fraction as variable formed.

The time step size provided is 0.0001 seconds and number of time steps is 1000 for all the cases.

Floating point exception error is a common problem in this simulation. The under relaxation can be reduced to check for the error.

The solution methods and the control parameters are:

 

•  Results:

This is a long simulation . Each case took nearly 6 hours to complete with my machine standards. The simulation with 20% n-heptane liquid is completely analysed . It completed 1000 time steps and the flow time recorded was  0.106 seconds . The scaled residuals will be pasted below.

 

The simulation link is provided below.

https://drive.google.com/file/d/1XXxeUyTKpYaxFHZu8-5SunVqqbqjO8ig/view?usp=sharing

Analysis:

The UDF when studied shows a rotational speed of 200 rad/s. This is the `omega`value. 

Equationg the relation,`omega=(2*pi*N)/(60)` 

It is seen that the 1 rotation takes a flow time of 0.0314 seconds.

In the above analysis, the flow time was 0.106 seconds,  so the number of rotations recorded is 3.37 times. It is good considering the academic license and the computational time . 

The other simulations were stopped midway , to save computational time. the scaled residuals and the simulation animatins are pasted below.

Scaled residuals for the simulation of engine oil 20%

Scaled residuals for engine oil 30%

Flow time recorded for engine oil was 

From this we can calculate the number of rotations as 2.77 

The simulation link is 

https://drive.google.com/file/d/1St1fU2vr1gK1M53-WQFoEIM9GIn_X1tF/view?usp=sharing

 

Animation videos and their links to google drive:

The animation link for The simulation using n-heptane and 20% is https://drive.google.com/file/d/1XXxeUyTKpYaxFHZu8-5SunVqqbqjO8ig/view?usp=sharing

The animation link for engine oil 20% is https://drive.google.com/file/d/15SvZ5Zth2izDyWgqbTtOetD42nEiRQVY/view?usp=sharing

The animation link for engine oil 30% is https://drive.google.com/file/d/1St1fU2vr1gK1M53-WQFoEIM9GIn_X1tF/view?usp=sharing

The simulation link for n-heptane 30% is https://drive.google.com/file/d/10z9mizRwe3-RSaAHnFnfnmjsS04EOvLI/view?usp=sharing

   

Snippets at two different iterations of the flow behaviour.

 General errors encountered:

1) negative cell volume:

When the boundary displacement is large compared to the local cell sizes, the cell quality can deteriorate or the cells can become degenerate. This will invalidate the mesh (e.g., result in negative cell volumes) and consequently, will lead to convergence problems when the solution is updated to the next time step. 

To control this , the time step size to be reduced.

2) Floating point exception:

The solver detects an arithmatic operation but cannot compute the same. Divergence is dealt with here.

ways to solve the error:

• Using under relaxation
• Using upwind solving schemes
• Limiting time step
• Checking mesh quality.

 

• Conclusion:

Generally in industries, 3D simulations are performed, Here 2D simulation is performed.

The number of rotations for which the simulation is studied in industries are 10-12 . here between 2 and 3 number of rotations are studied. 

Since the viscosity of n-heptane is less than that of engine oil, the flow of n-heptane is much more faster.

Since , from 20% to 30% the fluid volume increases, the fluid reaches more gear area.