Computational Fluid Dynamics Simulation of a Swimming Fish (Includes UDF)

      This post is about the simulation of a swimming fish. The fish body is made of NACA 0020 and 0015 aero-foils (air-foils). The fluke is made of NACA 0025 aero-foil (air-foil), as shown in Fig. 1. the CAD files with computational domain modelled around the fish is available here.

Fig. 1, The generic fish CAD model

      The motion of the fish's body is achieved using a combination of two user-defined functions (UDF). The UDFs use DEFINE_GRID_MOTION script mentioned below, for the head/front portion. This is taken from the ANSYS Fluent software manual, available in its original form here. The original UDF is modified for present use as required. To move the mesh, dynamic mesh option within ANSYS Fluent is enabled; with smoothing and re-meshing options. The period of oscillation is kept at 2.0 s. The Reynolds number of flow is kept at 100,000; which is typical for a swimming fish.

/**********************************************************

 node motion based on simple beam deflection equation

 compiled UDF

 **********************************************************/

#include "udf.h"

DEFINE_GRID_MOTION(undulating_head,domain,dt,time,dtime)

{

  Thread *tf = DT_THREAD(dt);

  face_t f;

  Node *v;

  real NV_VEC(omega), NV_VEC(axis), NV_VEC(dx);

  real NV_VEC(origin), NV_VEC(rvec);

  real sign;

  int n;

  

  /* set deforming flag on adjacent cell zone */

  SET_DEFORMING_THREAD_FLAG(THREAD_T0(tf));

  sign = 0.15707963267948966192313216916398 * cos (3.1415926535897932384626433832795 * time);

  

  Message ("time = %f, omega = %f\n", time, sign);

  

  NV_S(omega, =, 0.0);

  NV_D(axis, =, 0.0, 1.0, 0.0);

  NV_D(origin, =, 0.7, 0.0, 0.0);

  

  begin_f_loop(f,tf)

    {

      f_node_loop(f,tf,n)

        {

          v = F_NODE(f,tf,n);

          /* update node if x position is greater than 0.02

             and that the current node has not been previously

             visited when looping through previous faces */

          if (NODE_X(v) > 0.05 && NODE_X(v) < 0.7 && NODE_POS_NEED_UPDATE (v))

            {

              /* indicate that node position has been update

                 so that it's not updated more than once */

              NODE_POS_UPDATED(v);

              omega[1] = sign * pow (NODE_X(v), 0.5);

              NV_VV(rvec, =, NODE_COORD(v), -, origin);

              NV_CROSS(dx, omega, rvec);

              NV_S(dx, *=, dtime);

              NV_V(NODE_COORD(v), +=, dx);

            }

        }

    }

  end_f_loop(f,tf);

}

      The computational mesh, as shown in Fig. 2, uses cut-cell method with inflation layers. The mesh has 2,633,133 cells. The near wall y+ is kept at 5. The Spalart-Allmaras turbulence model is used to model the turbulence. The second order upwind scheme is used to discretize the momentum and modified turbulent viscosity equations. The time-step for this study is kept at 100th/period of oscillation.

Fig. 2, The mesh and zoom in view of the trailing edge.

      The animation showing fish motion is shown in Fig. 3. Within Fig. 3, the left side showcases the velocity iso-surfaces coloured by pressure and the vorticity iso-surfaces coloured by velocity magnitude is shown on the right.

Fig. 3, The animation.

      Another animation showing the fish motion is shown in Fig.4. Within Fig. 4, the left side shows surface pressure while the right side shows pressure iso-surfaces coloured by vorticity.

Fig. 4, The animation.

      If you want to collaborate on the research projects related to turbo-machinery, aerodynamics, renewable energy, please reach out. Thank you very much for reading.

Flying Wing Design using Computational Fluid Dynamics (Verification and Validation)

     This post is about a transient simulation of the ONERA M-6 flying-wing aircraft with a cross-section of ONERA D airfoil, as shown in Fig. 1.

Fig. 1, The simulated geometry. 

     The mesh had 2,474,614 cells in total with 300,892 cells on the wing surface, as shown in Fig. 2. The computational domain is shown in Fig. 4. The computational domain walls are at a distance equal to ten times the wingspan.

Fig. 2, The computational mesh.

Fig. 3, The computational domain.

     The simulated conditions are taken from [1-4] i.e. a freestream Mach number of 0.8395 at 101,325 Pa and 293.2 K. The angle of attack is 3.06°.

     The lift force from the present numerical simulation is at 19,551.65 N as compared to the lift force of 20,438.53 N as determined by [1-4]. The numerically determined drag force from present simulation is 1,370.88 N as compared to 1,313.24 N, as determined by [1-4].

     The results of lift and drag force from the present simulation are within 4.35% and 4.2% of the results calculated by NASA [4] and [1-3]. Streamlines and pressure surface plot around the aircraft surface are shown in Fig. 4.

Fig. 4, Results.

References

[1] Le Moigne, "A Discrete Navier-Stokes Adjoint Method for Aerodynamic Optimization of Blended Wing-Body, Configurations", PhD thesis, Cranfield University, United Kingdom, 2002.

[2] J. Lee, C. S. Kim, C. Kim, O. H. Rho, and K. D. Lee, "Parallelized Design Optimization for Transonic Wings using Aerodynamic Sensitivity Analysis", AIAA Paper 2002-0264, 2002.

[3] E. J. Neilsen and W. K. Anderson, "Recent Improvements in Aerodynamic Design Optimization on Unstructured Meshes", AIAA Paper 2001-0596, 2001.

[4] 3D ONERA M6 Wing Validation, https://turbmodels.larc.nasa.gov/onerawingnumerics_val_sa.html.

     Thank you for reading. If you would like to collaborate on research projects, 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.

Computational Fluid Dynamics Analysis of a Symmetrical Wing, Update 01

     This post is about the computational fluid dynamics analysis of a wing. The wing analyzed employed the NACA 0021 section throughout. The wing had a span of 4 m and a chord length of 1 m. The Reynolds number was kept at 3,000,000. The software employed was SolidWorks Flow Simulation Premium.

     The mesh had a total of 385,064 cells of which 84,826 cells were in contact with the wing surface, as shown in Fig. 1. The results are, indeed, mesh independent. Mesh controls were employed to refine the mesh near the wing surface. The computational domain employed was of cylindrical shape.

 

Fig. 1, The computational mesh around the wing.

 

     The velocity variation at various angles of attack around the wing cross-section is shown in Fig. 3 while the pressure variation on the wing surface is shown in Fig. 4. The results were validated against experiments conducted by [1].

 

Fig. 2, Velocity variation around the wing at 0-25 degree AOA, 5 degree increments.

 

Fig. 3, Pressure variation at the wing surface at 0-25 degree AOA, 5 degree increments.

     The purpose of this blog is maintain my online portfolio. I did this analysis because I realized I haven't written anything of this nature before. All of my previous simulations and/or blog entries were from the propulsion, renewable energy and turbo-machinery areas.
 

     Update 01

     CAD files are available here.

 

    
     Thank you for reading. If you would like to collaborate on research projects, please feel free to contact.

     [1] Fernando A. Rocha, Adson A. de Paula, Marcos d. Sousa, André V. Cavalieri, and Vitor G. Kleine, "Lift enhancement by wavy leading edges at Reynolds numbers between 700,000 and 3,000,000," Proceedings of the 2018 Applied Aerodynamics Conference, AIAA AVIATION Forum, Atlanta, GA, 2018.

     https://doi.org/10.2514/6.2018-3816

Wing with Leading Edge Tubercles: Update 01

Tubercles (bumps) added to the leading edge of the aeronautic wings are a class of vortex generators. As shown in the Figure 1.

Figure 1, Modified wing geometry

Figure 2, Baseline wing geometry

The wing's cross section is NACA 0012. The dimensions used for this analysis were as used by [Chen, J. H., S. S. Li, and V. T. Nguyen. "The effect of leading edge protuberances on the performance of small aspect ratio foils." 15th International Symposium on Flow Visualization. 2012]. The flow conditions were reproduced from the research paper mentioned. In the wing with the leading edge tubercles, the tubercle wavelength was kept at two-thirds of the wing span. The tubercle amplitude was kept at half of the wing chord.

Computational fluid dynamics analysis was conducted to analyze the effect of the leading edge tubercles on wing performance. For validation of the numerical methodology, the lift and drag produced by the wing was compared to the experiments conducted for the mentioned research paper at 25 degree angle of attack. The forces calculated using computational fluid dynamics were within 7.3 % and 1.4 % of the experimental values, respectively.

The addition of tubercles at the leading edge of a wing creates a non-uniform pressure distribution on the wing’s surface, as shown in Figure 3. This non uniform pressure distribution and the changed wing geometry is responsible for the creation of a counter rotating chord-wise vortex pair behind each tubercle trough, as shown in Figure 4. To read more about non uniform pressure distribution, refer to Non Uniform Pressure Distribution.

Figure 3, Non-uniform pressure distribution. L-R; Modified Wing, Baseline Wing

Figure 4, Counter-rotating chord-wise vortex formation. L-R; modified wing, baseline wing. Notice the absence of vortex structures, represented by circles in the modified wing, in the baseline wing.

These vortices re-energize the boundary layer between them by carrying high momentum flow close to the wing surface, as shown by the dynamic pressure distribution in Figure 5, which leads to a delay in stall for the wing with leading edge tubercles, as shown in Figure 6. It can be seen clearly from both Figure 5-6 that the flow is attached behind the tubercle crest in the wing with leading edge tubercles while the baseline wing had stalled completely. To read more, refer to Counter Rotating Chord-wise Vortex Formation and Reduction in the Blade Tip Vortices, Delayed Stall and Reduction in the Span-wise Flow.

Figure 5, Dynamic pressure distribution around the wings. Top; modified wing. L-R; tubercle crest, tubercle trough. Bottom; baseline wing, same span-wise locations where the tubercle crest and trough is for the modified wing.

Figure 6, Streamlines around the wings. L-R baseline wing, modified wing.

Another effect of adding the leading edge tubercles to the wing is reduced span-wise flow and wing-tip vortices. The reason for this is that the counter rotating chord-wise vortices generated as a result of adding tubercles to the wing geometry act as a barrier to any span-wise flow, as shown in Figure 7-8.

Figure 7, Velocity flow trajectories. L-R modified wing, baseline wing. Notice the reduced size and strength of the tip vortex for the modified wing in comparison with the baseline wing.

Figure 8, Streamlines on the surface of the wings. L-R; modified wing, baseline wing. Reduced span-wise flow, (T-B of the screen), is clearly visible in the modified wing.

Thank you for reading. I hope this post added to your knowledge about tubercles. Next up will be the results of the counter-rotating configuration for the NREL Phase VI wind turbine. For verification and validation of the said wind turbine numerical simulations, refer to Verification and Validation.

Some of the reviewed literature:

[1] Watts, P., and Fish, F. E., “The Influence of Passive, Leading Edge Tubercles on Wing Performance,” Proceedings of the Unmanned Untethered Submersible Technology (UUST01), 2001.

[2] Fernandes, Irelyn, Yogesh Sapkota, Tania Mammen, Atif Rasheed, Calvin Rebello, and Young H. Kim, "Theoretical and Experimental Investigation of Leading Edge Tubercles on the Wing Performance," Proceedings of the Aviation Technology, Integration, and Operations Conference, Los Angeles, CA, 2013.
doi.org/10.2514/6.2013-4300
[3] Frank E. Fish, Paul W. Weber, Mark M. Murray, Laurens E. Howle, “The Tubercles on Humpback Whales' Flippers: Application of Bio-Inspired Technology,” Integrative and Comparative Biology, Vol. 51, No. 1, 2011, pp. 203–213.
doi.org/10.1093/icb/icr016
[4] Pedro, H. T. C., and Kobayashi, M. H., “Numerical Study of Stall Delay on Humpback Whale Flippers,” 46th AIAA Aerospace Sciences Meeting and Exhibit, AIAA Paper 2008-0584, Reno, NV, 2008.
doi.org/10.2514/6.2008-584
[5] Fish, F. E., and Lauder, G. V., “Passive and Active Flow Control by Swimming Fishes and Mammals,” Annual Review of Fluid Mechanics, Vol. 38, 2006, pp. 193–224.
doi.org/10.1146/annurev.fluid.38.050304.092201
[6] Weber, P. W., Howle, L. E., Murray, M. M., & Miklosovic, D. S., “Computational Evaluation of the Performance of Lifting Surfaces with Leading-Edge Protuberances,” Journal of Aircraft, Vol. 48, No. 2, 2011, pp. 591-600.
doi.org/10.2514/1.C031163
[7] Miklosovic, D. S., Howle, L. E., Murray, M. M., & Frank E. Fish, “Leading-edge tubercles delay stall on humpback whale (Megaptera novaeangliae) flippers,” Physics of Fluids, Vol. 16, No. 5, 2004.
dx.doi.org/10.1063/1.1688341
[8] N. Rostamzadeh, K. L. Hansen, R. M. Kelso & B. B. Dally, “The formation mechanism and impact of streamwise vortices on NACA 0021 airfoil's performance with undulating leading edge modification,” Physics of Fluids, Vol. 26, No. 10, 2014.
dx.doi.org/10.1063/1.4896748
[9] K. L. Hansen, R. M. Kelso & B. B. Dally, “Performance Variations of Leading-Edge Tubercles for Distinct Airfoil Profiles,” AIAA Journal, Vol. 49, No. 1, 2011.
doi.org/10.2514/1.J050631
[10] Ernst A. van Nierop, Silas Alben, and Michael P. Brenner, “How Bumps on Whale Flippers Delay Stall: An Aerodynamic Model,” Physical Review Letters, Vol. 100, No. 5, 2008.
doi.org/10.1103/PhysRevLett.100.054502
[11] K.L. Hansen, R.M. Kelso, B.B. Dally, E.R. Hassan, “Analysis of the Streamwise Vortices Generated Between Leading Edge Tubercles,” Proceedings of 6th Australian Conference on Laser Diagnostics in Fluid Mechanics and Combustion, Canberra, 2011
[12] Shi, Weichao, Mehmet Atlar, Rosemary Norman, Batuhan Aktas, and Serkan Turkmen, "Numerical optimization and experimental validation for a tidal turbine blade with leading-edge tubercles," Renewable Energy, Vol. 96, Part A, 2016, pp. 42-55.
doi.org/10.1016/j.renene.2016.04.064
[13] Ri-Kui Zhang and Jie-Zhi Wu, “Aerodynamic characteristics of wind turbine blades with a sinusoidal leading edge,” Wind Energy, Vol. 15, No. 3, 2012, pp 407-424.
doi.org/10.1002/we.479
[14] Ibrahim, I. H., and T. H. New, "A numerical study on the effects of leading-edge modifications upon propeller flow characteristics," Proceedings of Ninth International Symposium on Turbulence and Shear Flow Phenomena. Melbourne, 2015.
[15] Moore, K., and A. Ning, "Aerodynamic Performance Characterization of Leading Edge Protrusions," 54th AIAA Aerospace Sciences Meeting, AIAA Paper 2016-1786, San Diego, CA, 2016.
doi.org/10.2514/6.2016-1786
[16] Ning, Zhe, and Hui Hu, "An Experimental Study on the Aerodynamics and Aeroacoustic Characteristics of Small Propellers of UAV," 54th AIAA Aerospace Sciences Meeting, AIAA Paper 2016-1785, San Diego, CA, 2016.
doi.org/10.2514/6.2016-1785

Update 01

Following are my publications relating to the subject of this post.

Butt, F.R., and Talha, T., "A Numerical Investigation of the Effect of Leading-Edge Tubercles on Propeller Performance," Journal of Aircraft. Vol. 56, No. 2 or No. 3, 2019, pp. XX. (Issue/page number(s) to assigned soon. Active DOI: https://arc.aiaa.org/doi/10.2514/1.C034845)

Butt, F.R., and Talha, T., "A Parametric Study of the Effect of the Leading-Edge Tubercles Geometry on the Performance of Aeronautic Propeller using Computational Fluid Dynamics (CFD)," Proceedings of the World Congress on Engineering, Vol. 2, Newswood Limited, Hong Kong, 2018, pp. 586-595, (active link: http://www.iaeng.org/publication/WCE2018/WCE2018_pp586-595.pdf).

Butt, F.R., and Talha, T., "Optimization of the Geometry and the Span-wise Positioning of the Leading-Edge Tubercles on a Helical Vertical-Axis Marine Turbine Blade ," AIAA Science and Technology Forum and Exposition 2019, Turbomachinery and Energy Systems, accepted for publication.

Comparison between Lift and Drag Produced by a Legacy Wing VS a Wing with Tubercles (Humpback Whale Fin's Inspired)

* Link for Plots (now showing here for some reason) http://3dimensionaldesigningandmanufacturing.blogspot.com/2015/07/plots-for-comparison-between-lift-and.html

Following data was obtained from the CFD Simulations carried out in SolidWorks Flow Simulation Premium.

Project: Design of a Wing/Blade with Tubercles for Airplanes and/or Turbines

Without Tubercles
Air Speed in Km/h	Lift in N	Drag in N
150	46.307	14.775
140	39.942	12.917
130	33.432	11.057
120	28.807	9.498
110	24.234	7.928
100	20.593	6.625
90	15.836	5.352
80	12.482	4.205
70	9.411	3.243
60	7.272	2.406
50	4.873	1.680
40	3.130	1.082
30	1.763	0.612
20	0.810	0.279
10	0.231	0.072

 

 

With Tubercles
Air Speed in Km/h	Lift in N	Drag in N
150	50.616	11.360
140	48.131	10.008
130	37.190	8.505
120	30.988	7.309
110	24.784	6.079
100	20.892	5.094
90	17.225	4.146
80	13.412	3.287
70	9.955	2.507
60	7.444	1.849
50	4.955	1.286
40	2.991	0.828
30	1.652	0.468
20	0.725	0.212
10	0.214	0.057

 

Comparison between Lift and Drag

Air Speed in Km/h	Percentage Less Drag		Percentage More Lift
150	23.113		8.513
140	22.520		17.014
130	23.080		10.105
120	22.974		7.038
110	23.322		2.219
100	23.109		1.431
90	22.534		8.064
80	21.831		6.934
70	22.695		5.465
60	23.150		2.311
50	23.452		1.655
40	23.475		-7.523
30	23.529		-6.719
20	24.014		-11.72
10	20.833		-7.94

 

It is clear that the wing with tubercles not only produces more lift at a particular velocity but also less drag.

Data for the Wing without Tubercles:

Wing Span: 1.07 m

Chord Length: 0.229 m

Air Velocity: 0-150 Km/h head on

Vertical Pitch: 0 Degree

Gravity Considered

Fluid: Dry Air at STP

Mesh Settings: Coarse (3/8)

Data for the Wing with Tubercles:

Wing Span: 1.067 m

Chord Length Large: 0.229 m

Chord Length Small: 0.203 m

Air Velocity: 0-150 Km/h head on

Vertical Pitch: 0 Degree

Gravity Considered

Fluid: Dry Air at STP

Mesh Settings: Coarse (3/8)

Let's now take a look at visual representation of data.

This Plot Shows Air Velocity VS Drag, Lift by the Wing without Tubercles

This Plot Shows Air Velocity VS Drag, Lift by the Wing with Tubercles

As you can see from above two plots; the wing with tubercles generates more lift and less drag.

This Plot Shows Air Velocity VS Lift Generated by the Wings

The green line represents the Lift generated by the wing with tubercles. It is between two to six percent more at each velocity.

This Plot Shows Air Velocity VS Drag Generated by the Wings

The green line represents the Drag generated by the wing with tubercles. It is around twenty two percent less at each velocity.

This Plot Shows Air velocity VS Lift to Drag Ratio

It is clear from this plot that Lift to Drag ratio of the wing with tubercles is around thirty three percent more for the wing without tubercles at a velocity point.

 

This Plot Shows Air Flow around the Wings at 150 Km/h from the Right Side

This Plot Shows Air Flow around the Wings at 150 Km/h

The Need for Tubercles

In aviation there are four forces at play, Lift which over comes Weight and Thrust which overcomes Drag. For a cruise speed at a particular altitude, three of these forces are almost constant. Our goal is to minimize Thrust, Drag and Weight and maximize Lift, this is because Thrust costs in terms of fuel flow rate and Weight and Drag negatively impacts on the agility of the aircraft. Aerodynamically efficient Wings and/or Blades with "Tubercles" will not only increase Lift and but also decrease Drag. This all means that we will need less Thrust for a cruise speed than before, that results in savings in terms of fuel which will result in healthier environment.

 

Applications:

 

Canal Turbine Concept

It's a concept I am currently working on, so far I gave made a CAD model (renderings attached) of it in SolidWorks and analyzed it using its built in CFD module.

There are many advantages of canal turbines over wind turbines, prominent one's being:

 

Unidirectional flow

Water flows in one direction in a canal so we don't need pitch and yaw control surfaces. That simplifies the design process and reduces weight.

Constant flow rate

We (humans) control water flow rate through canals and it's almost same all year, so we don't have to worry about blade aero foil design to suit variable/abruptly variable flow rate, that makes design process further straight forward.

Large Electricity potential

Canals are 100s of km long, imagine the electricity potential in the canals. You can put these turbines in irrigation canals and it'll power nearby villages and all the irrigation equipment etc.

Higher Power/Discharge Ratio

Water is ~816 times dense (powerful) than air, so for the same discharge (flow) rate we get potentially 816 times more power. Which means more we can make designs that are lighter, smaller and easier to manage and maintain.

Easy maintenance

Fitted less than ~1 m deep inside the canal and can be retracted for maintenance at ground level, making maintenance very easy or better yet, we can maintain them while canals are being cleaned.