Week 4 - Meshing for Fuselage Using Ansys ICEM
Objective:
Your challenge for this week is to create a domain suitable for the given helicopter fuselage geometry using ICEM CFD. The domain size is mentioned within the video i.e.
- Element size around the domain
- Prism element size
Calculate Y+, First cell height, Number of layers as explained in the video and apply it to the inflation layer.
Answer:
The half domain will be created becuase of symmetrical in nature.
The symmetry & farfield (for free stream velocity at infinity) boundary conditions will be applied. The farfield boundary condition will be applied to the side face, top face & bottom face. While the front face will be inlet & rear face will have outlet boundary condition.
Following flow conditions were considered for the simulation:
- Altitude of 4 km
- Free stream Mach number is 0.3
For meshing:
- Assume Y+ = 30
- Tetra mesh for farfield
- Prism mesh for boundary layer
Given Helocopter Fuselage Geometry
Characteristic Length
It is measured using measured distance tool.
After measuring characteristics length, the domain has been created as per below image.
To create this domain, first reference point has been created using the point creation tool given in ICEM user interface. To create point, the option called base point & delta option has been used. The first point has been created at a distance of 21808.35mm from the front reference point which is shown in the below image. In similar way, the other corner points of the domain has been created. The table following to below image is showing the inputs used to create the domain.
|
INDICATION |
TOTAL LENGTH (mm) |
|
C |
2423.15 |
|
9C |
21808.35 |
|
15C |
36347.25 |
|
10C |
24230.15 |
|
4.5C |
10904.17 |
Below image is showing all the reference points created using create point & transform tool.
After creating points all corner points, the lines has been crrated using the following option called Create/Modify Curve using points.
Next, surfaces have been creted using the create/modify surface option using simple surface method. From 2-4 curves option has been used from Simple Surface method as shown in below image.
Following is the domain created after generating surfaces.
Now to create the fluid domain, the option called create body has been used which will convert these seperate surfaces into one single body as a fluid which is shown into the image next to the below image. In that image, it can be seen as the fluid domain indicated.
In this fluid domain, the different areas are required to define as per their function like inlet, outlet, symmetry & far field areas. To define them, the option called Create Part has been used. In below image, the inlet has been created after selecting the front face. In a similar way, other parts were also defined.
Right now, the fuselage & fluid domain are two seperate entities. And because of that the solver will not be able to identify the fuselage in the fluid domain. To make define the fuselage as integral part of the fluid domain, the outer boundary of the fuselage will be trimmed from the fluid domain. To trim the boundary, the option called Segment/Trim Surface option available in Create/Modify Surface. The "Curve" method has been used in that option. The boundary was trimmed from the summetry surface.
After trimming from the symmetry surface, the fuselage surface was deleted using the "delete surface" option. The outcome is displayed in below image.
The final domain geometry was checked for any error using the Repair Geometry option. In that the option called, Build Diagnostic Topology option is used.
After applying, the boundary of the fluid domain became red which means there is no error involved in the geometry.
In next step, global mesh setup has been applied before creating mesh. To setup global mesh parameters, the first four options shown n the Global Mesh Parameters were applied to define the mesh. The first is Global Mesh Size shown in below image. The scale factor kept it at 1 & mesh element size was kept at 2048 mm.
The next option shell meshing parameters. All options were kept as by defualt.
After that Volume Meshing Parameters was defined for the Tetra/Prism mesh type. The Robust (Octree) mesh method was used to generate mesh because the prism layers are required to create in the mesh. The other method is "Quick (Delaunay)" method. This method is not used if requirement is to generate prism layers.
The fourth option is for the prism meshing parameters. In which the layers nearer to the fuselage boundary were created. The Initial height or first layer height & total height for 20 layers were calculated as per below analytical method.
The cell height depends on the following two conditions:
1. Type of flow
2. Turbulence model
If cell height (y+) has lower value than the higher resolution mesh & longer the solution time & vice versa.
To calculate initial cell height, following formula was used.
y+=ρUΔyμ">y+=ρUΔyμy+=ρUΔyμ
To implement this equation, the required inputs need to be calculated.
As per ISA, since the height is within 4 km, the lapse rate can be assumed as -6.5.
Temperature, T = 288.15 - 6.5 X 4 = 262.15 K
Speed of sound, a=γRT">a=√γRTa=γRT = sqrt(1.4 X 287 X 262.15) = 324.52 m/s
Free stream velocity, v = Mach Number X a = 0.3 X 324.52 = 97.36 m/s
According to ISA, Density, ρ=ρ0(ThT0)4.25">ρ=ρ0(ThT0)4.25ρ=ρ0(ThT0)4.25 = 1.225(262.15288.15)4.25">1.225(262.15288.15)4.251.225(262.15288.15)4.25 = 0.8195 kg/m^3
Viscosity, using Sutherland's law, μ=1.458⋅10-5⋅T1.5T+110.4">μ=1.458⋅10−5⋅T1.5T+110.4μ=1.458⋅10-5⋅T1.5T+110.4 = 1.661 X 10^-5 kg/ms
The first cell height has been calcualted using online y+ calculator provided by Pointwise. The result is as follows:
Now to calcualte the boundary layer height, following formula has beeb used.
δ=5⋅CRe">δ=5⋅C√Reδ=5⋅CRe = (5 X 2.422) / sqrt(11.6 X 10^6) = 3.556 X 10^-3 m
To calculate number of layers in the boundary layers = boundary layer height/ first cell height = 19.86
The calculated values have been inserted into the Prism Meshing parameters dialogue box.
After applying mesh parameters, the different mesh element lengths were assigned to the different part of the fluid domain. 32mm element length has been assigned to the parts of fuselage while the 512mm is assigned to the fluid domain parts.
The Density zone was created to generate finer mesh at the back of fuselage to capture the details.
The "Create Density" tool used to define the zone. The element size has been kept at 32mm which is far smaller than the global mesh element size of 2048mm.
Using transformation tool, the desnity zone was moved 1211 mm towards X direction.
At last mesh has been generated using Compute Mesh option.
Following image shows the generated mesh on the fluid domain.
The details of the generated mesh is as follows:
The mesh generated inside density zone is shown in below image. The elements are very fine compare to surrounding.
The certain mesh quality criterias were also used to determine the generated mesh accuracy.
Following four criterias were implemented:
1. Quality: For tetrahedral elements, it should be above 0.3 while for quadrihedral, above 0.4.
2. Determinant: It computes the presence of negative volume in the fluid domain. If the element volume is very low compare to the tolerance value set by the mesher than those elements will be considered as negative volumes. If solver encounters the negative volume during processing, it will consider it as error & stop proceeding further. 1 indicates perfect volume & 0 indicates bad volume. The negative indicates the presence of negative volume.
3. Aspect Ratio: It defines as the ratio of largest length to smallest length of the element. 1 means the perfect shape element.
4. Skewness: It indicates the deviation of element from equilateral shape. High skewness means less accurate results. The skewness value of 1 indicates highly degenerate while 0 means excellent.
The above criterias show that the improvement in the mesh is required as some elements still have the quality below 0.3, aspect ratio & skewnss are also required to improve.