Executive transport aircraft with truss-braced wing (World's First)

     To explore large-er aspect ratio wings; one fine morning, I just thought it would be fun to put a truss-braced wing in a Piaggio P.180 "Avanti". The modified design CAD files are is available here. A comparison is shown in Fig. 1. I am too lazy to make 2 separate airplanes so I modified half of it so I can run a CFD analysis using one model and one mesh 🤣. A slight modification about which I will write later is the positioning of the flaps and ailerons. These are moved to the truss part from the main wing in the original design. The aspect ratio is of the truss-braced section is double the original. With a foldable wing, storage shouldn't be a problem?

Fig. 1, Row 1, L-R Top, bottom; Row 2, L-R front, back; Row 3 L-R, left, right views

     Cruise conditions are taken from [1] i.e. ~12,500 m and ~163.6 m/s. The CFD mesh has 4,892,425 cells out of those, 449,732 are the the surface of the jet. I compare lift/drag of both halves. The modified section produces 36.15% more drag (force) as compared to the original design. The modified section however, produces 49% more lift (force) than the original design. L/D for truss-winged section is at 6.72 as compared to 6.14 for the original design. In terms of L/D, the truss-braced wing section produced 🥁 ... 9.45% more Lift/Drag. A resounding success 😁, I'd say. For validation of CFD, read this and this.

     Some post processing I did, is shown in Fig. 2. Velocity iso-lines with vectors are shown around the wings. Vorticity is shown in the wake of the jet(s). Tip vortex is smaller and less intense behind the truss-braced wing portion but there is another vortex where the truss meets with the main wing. In the main wing, for the trussed-braced portion; on the pressure side; the high pressure zones extend for a longer portion of the span in the span-wise direction as compared to the original design. Same is true for low pressure zones on the suction side of the main wing. Some day I will write a nice little paper and sent it to an AIAA conference, till then 𝌗.

Fig. 2, Colorful Fluid Dynamics 🌈

     Stream-wise vorticity is shown in Fig. 3. It is clear from Fig. 3 that the vorticity is less intense on the side with truss-braced wing as compared to the original design. Fig. 3 is colored by stream-wise velocity. The aircraft appears blue due to no slip condition.

Fig. 3, Some more Colorful Fluid Dynamics (CFD) 🌈

     Thank you for reading, if you would like to hire me as your master's / PhD student / post-doc / collaborate on research projects, please reach out! 😌

References

[1] "Operations Planning Guide". Business & Commercial Aviation. Aviation Week. May 2016. [https://web.archive.org/web/20160815060134/http://www.sellajet.com/adpages/BCA-2016.pdf]

High Lift Common Research Model (CRM-HL) CFD Simulation (with validation from Stanford CTR and NASA) Update 01: Formation Flight

     This post is about the CFD analysis of the nominal (2A) configuration of the Boeing / NASA CRM-HL with flap and slat angles at 40 and 37 degrees. The configuration is shown in Fig. 1.

Fig. 1, CRM-HL CAD

     The dimensions are mentioned in [1] and is available here and here. The numerical simulations are validated with published literature [3, 4]. SolidWorks Flow Simulation Premium software is employed for the CFD simulations. The flight conditions are Mach 0.2 at 289.444 K and 170093.66 Pa [2].

     Fig. 2 shows the computational mesh along with the computational domain. The surface mesh is also shown with Fig. 2. It can be seen that the mesh is refined in the areas of interests and in the wake of the aircraft to properly capture the relevant flow features. The Cartesian mesh with immersed boundary method, cut-cell approach and octree refinement is used for creating the mesh. The mesh has 6.5 million cells, of which around 0.71 millions cells are at boundary of the aircraft.

     The simulations employ κ-ε turbulence model with damping functions and two-scales wall functions. SIMPLE-R (modified) as the numerical algorithm. Second order upwind and central approximations as the spatial discretization schemes for the convective fluxes and diffusive terms. The software solves the Favre-averaged Navier-Stokes equations to predict turbulent flow. The simulations are performed to predict three-dimensional steady-state flow over the aircraft

Fig. 2, Dashed lines indicate symmetry boundary conditions

     Angle of attack of 7 and 17 degrees are considered. At 7 degree angle of attack, the drag life and moment coefficients are within 6, 8 and 12% of the published data, respectively. For 17 degree angle of attack, the coefficients are within 4, 7, 33% of the published data [3, 4]. On average, the results of the present simulations are within 6% of the published data for force coefficients and within 12% in terms of pitching moment coefficient. The pitching moment coefficient will improve with refinement of the mesh, as shown by [3]; which I will do if ever I convert this into a manuscript 😂. The post processing from CFD simulations is shown in Fig. 3-4. Within Fig. 3, the iso-surfaces represent vorticity in the direction of flow, colored by pressure. The direction of flow is shown by black arrows. Streamlines colored by vorticity are also visible. It can be seen from Fig. 2 that the simulation captures important flow features such as vortex formation very accurately, in such small number of mesh cells. Fig. 4 shows wing of the velocity iso-surfaces colored by vorticity in the direction of flow, focused around the wing.

Fig. 3, Alternating 7 and 17 degree angles of attacks

Fig. 4, Top-Bottom, 17 and 7 degrees angle of attack

     The simulations are solved using 10 of 12 threads of a 4.0 GHz CPU with 32 GB of total system memory of which almost 30 GB remains in use while the simulations are in progress. To solve each angle of attack, 3 hours and 47 minutes are required.

Update 01

     Formation flight simulation is performed with 7.3 million cells (limited by RAM). Symmetry boundary condition is used to simulate only the area of interest. The mesh and computational domain is shown in Fig. 5. Within Fig. 5, dashed lines indicate symmetry boundary condition.

Fig. 5, Airliners in formation flight mesh and computational domain

     The results show that the leading aircraft has 16.52% more drag than the trailing aircraft. The results also show that the the leading aircraft has 5.4% less lift than the trailing aircraft. However, the leading aircraft produces 2.4% more lift than the airliner flying without the trailing aircraft (flying solo). The leading aircraft also produces 3% less drag than the airliner flying solo. These results are at 7 degree angle of attack. Whether these results are fruitful aero-structurally, remains to be seen. The post processing from simulations are shown in Fig, 6.

Fig. 6, Top-Bottom, 17 and 7 degrees angle of attack

     Within Fig. 7, surface plots represent pressure, velocity streamlines indicate vortices, iso-surfaces show vorticity magnitude in the direction of flight.

     Thank you for reading, If you would like to collaborate on projects, please reach out.

References

[1] Doug Lacy and Adam M. Clark, "Definition of Initial Landing and Takeoff Reference Configurations for the High Lift Common Research Model (CRM-HL)", AIAA Aviation Forum, AIAA 2020-2771, 2020 10.2514/6.2020-2771

[2] 4th AIAA CFD High Lift Prediction Workshop Official Test Cases, https://hiliftpw.larc.nasa.gov/Workshop4/OfficialTestCases-HiLiftPW-4-2021_v15.pdf

[3] K. Goc, S., T. Bose and P. Moin, "Large-eddy simulation of the NASA high-lift common research model", Center for Turbulence Research, Stanford University, Annual Research Briefs 2021

[4] 4TH High Lift Workshop Results, ADS, https://new.aerodynamic-solutions.com/news/18

The Fan Car

     The idea to reduce Drag and/or improve Downforce on a vehicle using fans at the rear has been around for decades. Specially in the world of motorsports. Examples include Gordon Murray's BT46 and the T50. Here an explanation is made as to why placing a fan behind a car or a container-carrier truck can be used to improve fuel economy.

     The sample car model is of the renowned Ahmed Body. For validation of the numerical simulation, please refer to this post.

     Fig. 1 shows pressure isosurfaces around the car body both with and without fans installed at the rear. It is clear that the pressure difference between rear and front of the car is more when the fans are not available. More pressure difference results in more Drag and a relatively bad fuel economy.

Fig. 1, T-B; Fan disabled, fan enabled

     Fig. 2 shows cross section view of the car. It can be seen that the the boundary layer is re-energized and as a result the flow separation is significantly reduced by adding a fan at the rear. By adding a fan, the vortices are not only moved away from the rear-end of the car but also have smaller size and less intensity, as shown in Fig. 3.

Fig. 2, T-B; Fan disabled, fan enabled. Red arrows represent direction of airflow

Fig. 3, L-R; Fan disabled, fan enabled

Thank you for reading. Please share my work. If you would like to collaborate on a project please reach out.

High Camber Wing CFD Simulation

     This post is about the numerical simulation of a high camber, large aspect ratio wing. The wing had an aspect ratio of 5:1. The Reynolds number of flow was 500,000. The wing was at an angle of attack of zero degree. The aero-foil employed had a cross section of NACA 9410.

     The software employed was Flow Simulation Premium. A Cartesian mesh was created using the immersed boundary method. The mesh had 581,005 cells. Among those 581,005 cells, 55,882 were at the solid-fluid boundary. A time step of ~0.00528167 s was employed*. The domain was large enough to accurately trace the flow around the wing without any numerical or reversed flow errors. The software employs κ-ε turbulence model with damping functions, SIMPLE-R (modified) as the numerical algorithm and second order upwind and central approximations as the spatial discretization schemes for the convective fluxes and diffusive terms. The time derivatives are approximated with an implicit first-order Euler scheme.

     The mesh is shown in Fig. 1. The four layers of different mesh density are also visible in Fig. 1, the mesh is refined near the wing surface using a mesh control. The velocity around the wing section is shown in Fig. 2, using a cut plot at  the center of the wing. In Fig. 2, the wing body is super imposed by pressure plot. The velocity vectors showing the direction of flow are superimposed on both the wing body and the velocity cut plot.

Fig. 1, The computational domain.

Fig. 2, The velocity and pressure plots.

     The results of the simulation was validated against the results from XFLR5 software. XFLR5 predicted slightly higher lift and slightly less drag on the wing for same boundary conditions because the XFLR5 simulations were inviscid.

     Thank you for reading. If you would like to contribute to the research, both financially and scientifically, please feel free to reach out.

     *Time step is averaged because of the fact that a smaller time step was employed at the start of the numerical simulation.

SolidWorks Flow Simulation: Internal Variable Velocity Inlet Boundary Condition

     This post is about an internal computational fluid dynamics simulation. The Simulation was performed in a pipe with a diameter of 1 in. The length of the inlet was 8 in away from the intersection. The two outlets were 4 in away from the intersection and were at an angle of 120° from the inlet, respectively. The flow entered the pipe in pulses with a period of 0.2 s. The peak velocity was at 2 m/s and the minimum velocity was kept at 0 m/s. This simulation setup can be analogous to the opening/closing of an IC engine valve simulation or simulation of cardiovascular systems etc.

     The part used in the simulation and the simulation setup is available here, as shown in Fig. 1.

Fig. 1, Part geometry.

 

     The mesh is shown in Fig. 2. The simulation assumed 2D simplification, to save time and computational resources. The mesh had a total of 15,512 cells. A simulation time step of 0.00625 s was employed.

 

Fig. 2, The computational mesh.

 

     The velocity profile at 0.9 s is shown in Fig. 3.

 

Fig. 3, Velocity Streamlines colored by velocity magnitude, superimposed by velocity vectors.

 

     An animation of the results is shown below. The results are, indeed, mesh and time independent.

 

 

     Thank you for reading. Reach out to collaborate in research projects.

Wind Turbine SolidWorks Flow Simulation Premium Computational Fluid Dynamics: Verification and Validation

Numerical Methodology

Computational Fluid Dynamics analysis was performed using commercially available code SolidWorks Flow Simulation Premium© in the present study. SolidWorks Flow Simulation Premium© is a CAD embedded CFD tool; employs κ-ε turbulence model with damping functions, SIMPLE-R (modified) as the numerical algorithm and second order upwind and central approximations as the spatial discretization schemes for the convective fluxes and diffusive terms. The time derivatives are approximated with an implicit first-order Euler scheme. The Flow Simulation© solves the Navier-Stokes equations; mentioned below; which are formulations of mass and momentum conservation laws for fluid flows. To predict turbulent flows, the Favre-averaged Navier-Stokes equations are used.

∂ρ/∂t+∂(ρui)/∂xi=0

∂(ρui)/∂t+∂(ρuiuj)/∂xj+∂p/∂xi= ∂(τij+τijR)/∂xj+Si     i=1,2,3

where, Si is a mass-distributed external force per unit mass due to a porous media resistance (Siporous), a buoyancy (Sigravity=-ρgi is the gravitational acceleration component along the i-th coordinate direction) and the coordinate system’s rotation (Sirotation), i.e., Si=Siporous+Sigravity+Sirotation. The subscripts are used to denote summation over the three coordinate directions.

All the simulations were performed to predict three-dimensional transient flow over the wind turbine. The Local rotating region(s) (Sliding) feature within SolidWorks Flow Simulation Premium© software was employed to simulate the wind turbine’s rotation in standard atmosphere.

Validation and Verification

To ensure validation of the numerical methodology, the numerical results of the present study were compared with the experimental results. A total of six tip-speed ratios were selected for the present study, as mentioned in table 1. The NREL Phase VI wind turbine without contra-rotating technology was selected for validation and verification because there is no reliable experimental data available for the NREL Phase VI wind turbine incorporating the contra rotating technology. The operating rotational velocity for the NREL Phase VI wind turbine is 7.5 rad.s-1. The diameter of the wind turbine is 10.058 m.

Table 1; TSR and the corresponding wind speeds

TSR	Wind Speed [ms-1]
7.5	5
5.03	7.5
3.77	10
3.02	12.5
2.52	15
1.89	20

The comparison between the experimentally determined shaft torques and numerical results of the present study, along with the number of mesh cells and the time step employed at various wind speeds is shown in table 2. A comparison of the present study with other studies conducted on the NREL Phase VI wind turbine is presented in Figure 1.

The computational domain selected had a size of 4Dx4Dx2.8D. The computational domain had a large enough volume to accurately trace the fluid flow around the wind turbine and for the solver to operate without any reversed flow or unwanted vortex formation or any other numerical difficulties.

Flow Simulation© considers the real model created within SolidWorks© and automatically generates a Cartesian computational mesh in the computational domain distinguishing the fluid and solid domains. The resulting mesh, employs the immersed boundary method, has three types of cells, namely Fluid cells; the cells located entirely in the fluid, Solid cells; the cells located entirely in the solid and Partial cells are the cells which are partly in the solid and partly in the fluid [22]. The Cartesian mesh with immersed boundary method has certain advantages, like the mesh is very quick to generate and results in high quality elements. The solution converges faster and the mesh distortion and numerical errors are relatively lower. During the process of mesh generation, it was made sure that the region of interest; the region immediately surrounding the wind turbine; had a very fine mesh as compared to the boundaries of the computational domain, to make the simulations converge. The Local Mesh option within the SolidWorks Flow Simulation Premium© software was employed to increase the mesh density in the critical areas.

Table 2; Comparison of the Experimental and Numerical Results

Wind Speed [ms-1]	Experimental Power [W]	Numerical Power [W]	Percentage Difference	Mesh Cells [x105]	Time Step [x10-3 s]
5	2,000	2,043	2.1	3.77	5.41
7.5	6,000	6,105	1.72	3.77	5.41
10	10,000	10,230	2.25	3.77	5.41
12.5	9,500	9,343	1.65	7.79	1.9
15	9,000	7,606	15.49	7.79	1.9
20	8,500	8,696	2.25	9.21	1.96

Figure 1; Comparison of results from present study with previous works

Project Files and Illustrations
     The project files are available here. An illustration of the rotor is provided below.

CFD Post Processing