Saithe Fish Simulation: ANSYS Fluent Dynamic Mesh Setup

     One of the most famous post on the blog can be read here. Worryingly😁, many fellow researchers and readers are interested in the aerodynamics of flexible robots 🤓. In this post, the dynamic mesh 🕸 settings used are shared 🥰. These settings are used to reproduce 🖨️ the results from [1], all those years ago. All in a hope that this post helps the readers in their scholarly work! 🎩

     Once the UDF 💻 has been acquired, the next step is to apply the UDF to the airfoil 🐠 geometry correctly ✔️. The airfoil geometry at the first time-step 🕰 i.e. at t = 0 for UDF 02 obtained from [1] is made available here. Once on the dynamic 🏎️ mesh page, select the options shown in Fig. 1. The options selected in Fig. 1 show the default parameters. Within Fig. 1, "wing" refers to the named selection that includes the only the airfoil geometry. Named selections can be created during the meshing process. The "wing" named selection is shown in Fig. 3.

Fig. 1, The dynamic mesh settings

     Before following the settings in Fig. 1, do remember to compile the UDF. To compile the UDF, please use the settings shown in Fig. 2. After selecting the UDF, select the options as shown in the Fig. 2 and then select Build and Load.

Fig. 2, Compile UDF

Fig. 3, Named selection for the dynamic mesh

     The maximum Lift ⬆️ force coefficient from the simulations performed using the method explained here is at 1.77 as compared to 1.68 [1]. The average Drag ⬅️ coefficient is at 0.097 as compared to 0.103 [1]. The obtained flow-field 🏟️ is shown in Fig. 4. Within Fig. 4, top row has v and u components of velocity while the bottom row shows pressure field❗

Fig. 4, The flow-field

     If you are still having trouble 😟, switch to immersed 🛀 boundary method. The immersed boundary method code yours truly wrote 🤓, is available here. Of course, this was done in abundant spare time 🕰️. The validation of this code is available here, here, here and more generally here 😼.

     If you want to hire me as your next shining post-doc or collaborate in research, please reach out! Thank you for reading!

References

[1] Shi, Fulong, Xin, Jianjian and Ou, Chuanzhong, Li, Zhiwei, Chang, Xing, Wan, Ling, "Effects of the Reynolds number and attack angle on wake dynamics of fish swimming in oblique flows", Physics of Fluids, 37(2), 025205, 2025 https://doi.org/10.1063/5.0252506 

Saithe Fish UDF (ANSYS Fluent)

     This post is about Fish Simulation in ANSYS Fluent using a User Defined Function (UDF). The UDF is mentioned below. The flow conditions are taken from [1]. This goes with the videos shown in Fig. 1-2. The CAD files for t=0 are available here (for UDF 01). A tutorial is available here.

Fig. 1, Animation of motion achieved through the UDF 01.

 

 Fig. 2, Animation of motion achieved through the UDF 02 (Validated).

     The results of present simulations are compared with [1]. The results are in excellent agreement as the C_{l, max} from [1] is at 1.57 while the maximum C_{l, max} from present simulation is at 1.6. The drag coefficient [1], C_{d, max} in [1] is at 0.164; while from the present simulations I got, 0.151. The C_{d, avg} comes out to be 0.072 [1] form the present simulations. I got a value of 0.064 from he present simulation. These would gradually become more accurate with mesh refinement, which I will certainly do if I send some ideas I have for peer review.

UDF 01:

#include "udf.h"

#include "unsteady.h"

#include "dynamesh_tools.h"

#include "math.h"

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

{

 Thread *tf = DT_THREAD(dt);

 face_t f;

 Node *v;

 int n;

 double x, y, y_ref_previous, y_ref;

 SET_DEFORMING_THREAD_FLAG(THREAD_T0(tf));  

 begin_f_loop(f,tf) {

  f_node_loop(f,tf,n) {

   v = F_NODE(f,tf,n);

   if (NODE_POS_NEED_UPDATE(v)) {

    NODE_POS_UPDATED(v);

    x = NODE_X(v);

    real amplitude = 0.02 + 0.01*x + 0.1*x*x;

    y_ref_previous = amplitude * cos(2*M_PI*x + 2*M_PI*0.8*(PREVIOUS_TIME));

    y_ref = amplitude * cos(2*M_PI*x + 2*M_PI*0.8*(CURRENT_TIME));

     

if (NODE_Y(v) > y_ref_previous){

     NODE_Y(v) = y_ref+fabs(NODE_Y(v)-y_ref_previous);

    }

    else 

     if (NODE_Y(v) < y_ref_previous){

      NODE_Y(v) = y_ref-fabs(NODE_Y(v)-y_ref_previous);

     }

     else {

      NODE_Y(v) = y_ref;

     }

    }

   }

  }

 }

 end_f_loop(f,tf);

UDF 02 (Validated):

#include "udf.h"

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

{

 Thread *tf = DT_THREAD(dt);

 face_t f;

 Node *v;

 int n;

 double x, y_ref_previous, y_ref, amplitude, fr;

 SET_DEFORMING_THREAD_FLAG(THREAD_T0(tf));  

 begin_f_loop(f,tf) {

  f_node_loop(f,tf,n) {

   v = F_NODE(f,tf,n);

   if (NODE_POS_NEED_UPDATE(v)) {

    NODE_POS_UPDATED(v);

    x = fabs(NODE_X(v));

    amplitude = 0.02 - 0.0825 * x + 0.1625 * x * x;

    fr = 2;

    y_ref_previous = amplitude * cos(2 * M_PI * x - 2 * M_PI * fr * (PREVIOUS_TIME));

    y_ref = amplitude * cos(2 * M_PI * x - 2 * M_PI * fr * (CURRENT_TIME));

     

if (NODE_Y(v) > y_ref_previous){

     NODE_Y(v) = y_ref + fabs(NODE_Y(v) - y_ref_previous);

    }

    else 

     if (NODE_Y(v) < y_ref_previous){

      NODE_Y(v) = y_ref - fabs(NODE_Y(v) - y_ref_previous);

     }

     else {

      NODE_Y(v) = y_ref;

     }

    }

   }

  }

 }

 end_f_loop(f,tf);

If you want to hire me as you next shining PhD/Master student or collaborate in research, please reach out! Thank you for reading!

References

[1] Gen-Jin Dong, Xi-Yun Lu; Characteristics of flow over traveling wavy foils in a side-by-side arrangement. Physics of Fluids 1 May 2007; 19 (5): 057107. https://doi.org/10.1063/1.2736083

Datacenter Visualization (Verified and Validated)

     This simulation is done to create an aero-thermal digital twin of a datacenter using CFD. The details of datacenter are taken from [1]. The datacenter CAD model is shown in Fig. 1.

     The simulation 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. Flow simulation solves the Navier–Stokes equations, which are formulations of mass, momentum, and energy conservation laws for fluid flows. To predict turbulent flows, the Favre-averaged Navier–Stokes equations are used.

Fig. 1, Datacenter CAD

     A Cartesian mesh with octree refinement, cut-cell method and immersed boundary methods is used. Special mesh refinements are deployed in the areas of interest i.e. inlets and outlets and sharp edges of server racks and CRAH units to accurately capture aero-thermal gradients and vortices. The resulting computational mesh has 2,698,156 cells. The computational domain and mesh are shown in Fig. 2.

Fig. 2, Computational mesh and domain

     The results from the numerical analysis were compared with [1]. The results are in excellent agreement with previously published data. The animation in Fig. 3 shows thermal distribution inside datacenter using cut-plots. Fluid velocity distribution is also shown. The cut-plots are superimposed with streamlines and velocity vectors. These post processing features help identify hot-spots and recirculation zones. Design improvements can be made to reduce thee unwanted flow features. Within Fig. 3, Flow trajectories colored by air temperature are also shown. These show path the fluid takes between various inlets and outlets in the datacenter such as the CRAH system supply and return zones and inlets and outlets of servers. Fig. 4 shows various post processing tools available for diagnosing various issues from the aero-thermal perspective. These include iso-surfaces, cut-plots, flow trajectories and surface plots etc.

Fig. 3, The post processing animations

Fig. 4, The post processing images

     A comparison of the results from present simulations with previously published literature is shown in Fig. 5. it can be seen that out results are in close agreement with previously published numerical and experimental data [1]! The locations at which the data is extracted is shown in Fig. 6. Within Fig. 5, solid lines indicate present study, dashed lines indicate published numerical results and filled circles represent published experimental results.

Fig. 5, Comparison of results

Fig. 6, Location of data extraction

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

References

[1] Wibron, Emelie, Anna-Lena Ljung, and T. Staffan Lundström. 2018. "Computational Fluid Dynamics Modeling and Validating Experiments of Airflow in a Data Center" Energies 11, no. 3: 644. https://doi.org/10.3390/en11030644

Heaving Airfoil Simulation

This post is about a 2D NACA 0012 heaving aerofoil. Heaving motion is achieved by changing the angle of attack on the aerofoil based on the Eqn. 1.

α_e = arctan[2*π*St_a*cos(2*π*f_h*t)]+ α_i               Eqn. 1

w.r.t. Eqn. 1, α_e is the effective angle of attack, St_a is Strouhal number, f_h is the heaving frequency.

The case S1 and H6 from [1] are compared in the animations below.

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

References

[1] https://doi.org/10.1121/10.0001419