Learning Forum

[Kanak BUET19]

Hello everyone,

I am trying to simulate Selective Laser Melting in Ansys Fluent. Its a two phase problem. So I am using VOF model.

my domain dimension is :

L = 0.8 mm (X axis)
W = 0.2 mm (Y axis)
H = 0.28 mm (Z axis)

In this domain , I patched the domain ( x = 0.8 mm, y = 0.2 mm , z= 0.2 mm) as solid and the rest is gas.

I am trying to model the heat source as surface heat source and place it at x = 0 mm , y = 0.1 mm and z is undefined as I will use if statement to find the interface ( where 0
My UDF code is given below. After Compiling and initialising , when I try to view the user defined volumetric heat source under the contour tab , FLUENT Crashes instantly. I am not sure what went wrong. Yes I also created 5 user defined memory locations. Can anyone help?

#include "udf.h"
#include "sg_mphase.h"
#include "mem.h"
#include "sg_mem.h"
#include "math.h"
#include "flow.h"
#include "unsteady.h"
#include "metric.h"

// Constants
#define A 0.4 // Absorption coefficient
#define P 200 // Laser power (W)
#define R 40e-6 // Spot radius (m)
#define v 0.5 // Scan speed of laser (m/s)
#define Pi 3.1415926535 // Pi constant
#define x0 0.0 // Initial x position of the laser (m)
#define y0 0.1e-3 // Initial y position of the laser (m)

// UDF for adjusting the gradient heat
DEFINE_ADJUST(adjust_gradient_heat, domain)
{
Thread *t;
Thread **pt;
cell_t c;
int phase_domain_index = 3.0; // thjats my metal domain
Domain *pDomain = DOMAIN_SUB_DOMAIN(domain, phase_domain_index);

Alloc_Storage_Vars(pDomain, SV_VOF_RG, SV_VOF_G, SV_NULL);
Scalar_Reconstruction(pDomain, SV_VOF, -1, SV_VOF_RG, NULL);
Scalar_Derivatives(pDomain, SV_VOF, -1, SV_VOF_G, SV_VOF_RG, Vof_Deriv_Accumulate);

mp_thread_loop_c(t, domain, pt)
if (FLUID_THREAD_P(t))
{
Thread *ppt = pt[phase_domain_index];

begin_c_loop(c, t)
{
C_UDMI(c, t, 0) = C_VOF_G(c, ppt)[0];
C_UDMI(c, t, 1) = C_VOF_G(c, ppt)[1];
C_UDMI(c, t, 2) = C_VOF_G(c, ppt)[2];
C_UDMI(c, t, 3) = sqrt(C_UDMI(c, t, 0) * C_UDMI(c, t, 0) +
C_UDMI(c, t, 1) * C_UDMI(c, t, 1) +
C_UDMI(c, t, 2) * C_UDMI(c, t, 2)); // Magnitude of gradient of volume fraction

}
end_c_loop(c, t)
}

Free_Storage_Vars(pDomain, SV_VOF_RG, SV_VOF_G, SV_NULL);
}

// UDF for defining the heat source
DEFINE_SOURCE(heat_source, c, t, dS, eqn)
{
Thread *pri_th; // Gas phase
Thread *sec_th; // solid phase
real source;
real x[ND_ND], time;
time = CURRENT_TIME; // Acquire time from Fluent solver
C_CENTROID(x, c, t); // Acquire the cell centroid location
real T = C_T(c, t);

pri_th = THREAD_SUB_THREAD(t, 0);
sec_th = THREAD_SUB_THREAD(t, 1);





real rho = C_R(c,t);
real Cp = C_CP(c,t);

real rhom = C_R(c,sec_th);
real Cpm = C_CP(c,sec_th);

real rhog = C_R(c,pri_th);
real Cpg = C_CP(c,pri_th);
real factor = (2 * rho * Cp) / (rhom * Cpm + rhog * Cpg);

real r = sqrt(pow(x[0] - x0 - v * time, 2.0) + pow(x[1] - y0, 2.0));

if (C_VOF(c, t) > 0.05 && C_VOF(c, t) < 1)
{
source = ((2 * A * P) / (Pi * R * R)) * exp((-2 * (r * r)) / (R * R))*factor * C_UDMI(c,t,3);
dS[eqn] = 0.0;
}
else
{
source = 0.0;
dS[eqn] = 0.0;
}

return source;
}

[Rob]

What if a gradient is negative? 

[Kanak BUET19]

Even if the gradient is negative , I am squaring and rooting the x,y,z gradients and adding them in UDMI 3 right? It aint supposed to be the issue. However when I tried writing the heat source using DEFINE_PROFILE and used begin_f_loop , it worked (although I couldnt add any multiplying factor and gradient UDMI) . I need to multiply the "factor" and "UDMI" in order to convert the surface heat source to volumetric heat source.

 

CODE : ( This heats up both my gasesous and solid phase , which I dont want)

 

#include "udf.h"

DEFINE_PROFILE(heat_source_profile, thread, position)

{

    real x[ND_ND];

    face_t f;

    real current_time;

    real Q = 120; // Define your heat source magnitude (Watts)

    real rx = 5.3e-5; // Define your desired values for rx, ry, rz (meters)

    real ry = 250e-6;

    real rz = 5.3e-5;

    real A;

    real vel = 0.1e-3; // velocity @ m/s

    real PI = 3.1416;

    real x_pos;

    real x_start = 0; // Set your desired starting position in x (m)

    real y_start = 0.2e-3; // Set your desired starting position in y (m)

    real z_start = 0.1e-3; // Set your desired starting position in z (m)

 

   

    real x_local, y_local, z_local; // Declare local coordinates

 

   

    current_time = CURRENT_TIME;

    A = (6 * sqrt(3) * Q) / (PI * sqrt(PI) * rx * ry * rz);

    x_local = 0.0; // Initialize x_local outside the loop

    y_local = 0.0; // Initialize y_local outside the loop

    z_local = 0.0; // Initialize z_local outside the loop

   

    begin_f_loop(f, thread)

    {

        F_CENTROID(x, f, thread);

       

        // Transform global coordinates to local coordinates

        x_local = x[0] - x_start;

        y_local = x[1] - y_start;

        z_local = x[2] - z_start;

       

        x_pos = vel * current_time;

     

       

       

        // Compute the heat source function value

       

         F_PROFILE(f, thread, position) = A * exp(-3 * (pow(x_local - x_pos, 2.) / pow(rx, 2.) + pow(y_local, 2.) / pow(ry, 2.) + pow(z_local, 2.) / pow(rz, 2.)));

         

         

    }

    end_f_loop(f, thread)

}

[Rob]

How would a face loop work on a VOF free surface?

[Kanak BUET19]

 

I have no idea sir :)) But I have worked something out :

I have run the code ( added below) and the heat source part perfectly worked out ( i.e its being applied to where 0

Code : 

 

#include “udf.h”

#include “sg_mphase.h”

#include “mem.h”

#include “sg_mem.h”

#include “math.h”

#include “flow.h”

#include “unsteady.h”

#include “metric.h”

// Constants

#define A 0.4 // Absorption coefficient

#define P 200 // Laser power (W)

#define R 40e-6 // Spot radius (m)

#define v 0.5 // Scan speed of laser (m/s)

#define Pi 3.1415926535 // Pi constant

#define x0 0.2e-3 // Initial x position of the laser (m)

#define y0 0.1e-3 // Initial y position of the laser (m)

#include “udf.h”

#include “sg_mphase.h”

#include “mem.h”

#include “sg_mem.h”

#include “math.h”

#include “flow.h”

#include “unsteady.h”

#include “metric.h”

// UDF for adjusting the gradient heat

DEFINE_ADJUST(adjust_gradient_heat, domain)

{

Thread *t;

Thread **pt;

cell_t c;

int phase_domain_index = 3.0; // thjats my metal domain

Domain *pDomain = DOMAIN_SUB_DOMAIN(domain, phase_domain_index);

Alloc_Storage_Vars(pDomain, SV_VOF_RG, SV_VOF_G, SV_NULL);

Scalar_Reconstruction(pDomain, SV_VOF, -1, SV_VOF_RG, NULL);

Scalar_Derivatives(pDomain, SV_VOF, -1, SV_VOF_G, SV_VOF_RG, Vof_Deriv_Accumulate);

mp_thread_loop_c(t, domain, pt)

if (FLUID_THREAD_P(t))

{

    Thread *ppt = pt[phase_domain_index];

    begin_c_loop(c, t)

    {

    C_UDMI(c, t, 0) = C_VOF_G(c, ppt)[0];

    C_UDMI(c, t, 1) = C_VOF_G(c, ppt)[1];

    C_UDMI(c, t, 2) = C_VOF_G(c, ppt)[2];

    C_UDMI(c, t, 3) = sqrt(C_UDMI(c, t, 0) * C_UDMI(c, t, 0) + C_UDMI(c, t, 1) * C_UDMI(c, t, 1) + C_UDMI(c, t, 2) * C_UDMI(c, t, 2)); // Magnitude of gradient of volume fraction

    }

    end_c_loop(c, t)

    }

    Free_Storage_Vars(pDomain, SV_VOF_RG, SV_VOF_G, SV_NULL);

}

// UDF for defining the heat source

DEFINE_SOURCE(heat_source, c, t, dS, eqn)

{

Thread *pri_th; // Gas phase

Thread *sec_th; // solid phase

real source = 0.0 ;

real x[ND_ND], time;

time = CURRENT_TIME; // Acquire time from Fluent solver

C_CENTROID(x, c, t); // Acquire the cell centroid location

real T = C_T(c, t);

pri_th = THREAD_SUB_THREAD(t, 0);

sec_th = THREAD_SUB_THREAD(t, 1);

real rho = C_R(c,t);

real Cp = C_CP(c,t);

real rhom = C_R(c,sec_th);

real Cpm = C_CP(c,sec_th);

real rhog = C_R(c,pri_th);

real Cpg = C_CP(c,pri_th);

real factor = (2 * rho * Cp) / (rhom * Cpm + rhog * Cpg);

Message(“Factor = %f\n”,factor);

real r = sqrt(pow(x[0] – x0 – v * time, 2.0) + pow(x[1] – y0, 2.0));

if (C_VOF(c, sec_th) > 0.05 && C_VOF(c, sec_th) < 1)

{

source = ((2 * A * P) / (Pi * R * R)) * exp((-2 * (r * r)) / (R * R))*factor ;

dS[eqn] = 0.0;

}

else

{

source = 0.0;

dS[eqn] = 0.0;

}

return source;

}

 

[Kanak BUET19]

Sorry Something went wrong . I said that , The volume fraction gradient calculation isnt working. Everytime i multiply the term C_UDMI(c,t,2) with source,  result becomes 0 . Any chance I might have done any mistake in the DEFINE_ADJUST part?

[Rob]

No idea as I don't do much coding and we don't debug. Why not just use the gradients directly? 

[Kanak BUET19]

In my code, I am taking value of  C_VOF_G . Apparently it seems in order for this to work , I need to set : solve/set/expert/Keep temporary solver memory from being feed? to YES

but, upon doing this I found this message : 

Info: Expert option for not freeing temporary solver memory is incompatible with adaption in parallel. 

(Also I have used mesh adaption to patch solid domain )

Since, fluent doesnt work in serial in recent days, I need your guidance for storing the VOF Gradient value somehow. Any suggestions? 

[Rob]

You may have created a register, unless you've set refinement/coarsening you've not adapted the model so you should be OK. 

[Kanak BUET19]

Yes I have created a register and I am obliged to do that for my simulation purpose. As I mentioned earlier, I needed to patch the solid domain to define two different phases. But now I need to calculate VOF gradient of the solid phase. Is there any other way to obtain VOF_G ? 

[Rob]

Have you tried running the solver with the code? 

[Kanak BUET19]

All this time I was just checking the contour after initialising. Never really bothered to run the simulation . After running , initially the Gradient was 0 but as soon as I started the sim , it started working!!! THANKS A LOT ROB!! Love you <3

[Rob]

You'll find some of the UDF calls come at start/end of a time step so it's always worth running before checking output values. 

[Kanak BUET19]

 

Hi Rob, 

 

Thanks for the earlier suggestions. I have finally been able to run the simulation and also been able to visualize the meltpool. (added below) 

 

I still haven’t added the Marangoni force equation yet. and for that I need to use temperature gradient value. But I am facing a problem. 

 

Here’s a brief summary of my problem : 

 

When inside the DEFINE_ADJUST function , I try to add this following line : 

 

C_TEMP_G_X(c,t) = C_T_G(c,t)[0] ; 

 

After running the simulation fluent crashes instantly. Basically I have renamed the UDMI earlier and now trying to apply the gradient on that UDMI . Any suggestions why is it happening?

 

NOTE : I have alloted sufficient UDMI mannually in the GUI 

 

I renamed it like that : 

 

#include “udf.h”

…..

…..

 

#define C_TEMP_G_X(c, t) C_UDMI(c, t, 8) // Renaming the UDMI 

 

DEFINE_ADJUST(adjust_gradient_heat, domain)

{

… ….

C_TEMP_G_X(c,t) = C_T_G(c,t)[0] ; // Applying X axis temp gradient into the renamed UDMI 

 

 

}

 

 

 

 

 

 

[Rob]

Does it work if you just use C_UDMI = C_T  with all of the (c,t) bits?  Making up labels that are similar to something Fluent may use can be a little risky. 

[Kanak BUET19]

I actually figured out the problem. The issue was I forgot to add the below portion inside the DEFINE_ADJUST code. Thanks though ! 

 

Alloc_Storage_Vars(domain, SV_T_RG, SV_T_G, SV_NULL);

T_derivatives(domain);

Free_Storage_Vars(domain, SV_T_RG, SV_NULL);