[fshak92]

I want to simulate the thermal effect of a laser beam(which is moving) on a multiphase surface.
I would appreciate if anyone has ideas about the way(s) i can simulate the moving laser beam.(In Star-CCM+ and/or Ansys and/or OpenFOAM)

Thank you in advance.

[fshak92]

I've tried to do a sample Solid case,by defining a table with the moving heat flux according to time.

a) Im not sure it will be the correct way to set a defined heat flux to the fixed coordinates in multiphase case.

b) Making a table to simulate the moving heat flux, somehow is time consuming.Because i should change the heat flux in each coordinates and each time step.(Below is a sample version of table i've used)

x y z t(1s) t(2s) t(3s) ...
1 0 0 500 0 0
2 0 0 0 500 0
3 0 0 0 0 500
.
.
.

Do you have any idea or suggestion about 'a' and 'b' ?
Thank you in advance.

[fshak92]

Nobody has any idea?

[flotus1]

I am currently busy with quite a similar project. In my case, it is not a multiphase problem.

I am using Ansys fluent for the simulations, since the definition of the transient boundary condition is quite simple there.

If you want to switch to fluent, maybe we could join forces.

[fshak92]

Originally Posted by flotus1

I am currently busy with quite a similar project. In my case, it is not a multiphase problem.

I am using Assys fluent for the simulations, since the definition of the transient boundary condition is quite simple there.

If you want to switch to fluent, maybe we could join forces.

Thank you for your reply.
Yes i can access to Ansys fluent,Would you please tell me how you did it?or please tell me some keywords about the way ,then i can find more explanation in user guide...

[flotus1]

If your boundary condition is just a heat flux, then set the BoCo to "wall" and apply a User Defined Function (UDF) as the thermal condition.
A UDF is a text file wit a .c extension which can be interpreted by fluent directly.

For a simplified 2-dimensional case with the laser beam moving in x-direction and having a rectangular intensity distribution, the UDF might look like this:

#include "udf.h"

DEFINE_PROFILE(laser_beam,t,i)                //Randbedingung für den Energiefluss durch den Laser
{
    real x[ND_ND];                   //Ortsvektor; ND liest aus ob 2D oder 3D-Fall
    real X;                             //Ortskoordinate
    real x_0=0.05;                   //starting point
    real v=0.05;                     //velocity of the laser beam
    real b=0.005;                    //width of the laser beam
    real I_0=50000000;            //Intensity
    real time=RP_Get_Real("flow-time");        //der Variable time wird die Simulationszeit zugewiesen
    face_t f;
    begin_f_loop(f,t)
    {
        F_CENTROID(x,f,t);            //liest Koordinate aus
        X=x[0];
        if(X>=x_0+time*v-b/2 && X<=x_0+time*v+b/2)    //Laser bewegt sich entlang X
            F_PROFILE(f,t,i) = I_0;
        else
            F_PROFILE(f,t,i) = 0;
    }
    end_f_loop(f,t);
}

Put the code in a text file, for example beam.c
In Fluent, go to "define" - "user defined" - "functions" - "interpreted" and choose the file. Click on "Interpret".
Now when setting up the heat flux for the boundary condition, the drop down menu which reads "constant" should allow picking the "laser_beam" profile defined in the UDF.

Since I want to simulate melting of the material by the laser, I am no longer using a heat flux as a boundary condition. Instead, I am trying to use the Discrete Ordinates radiation model to simulate the laser beam.
But if you just want to heat up the material, a heat flux BoCo should be sufficient.

[fshak92]

Many Many Thanks to you indeed:-)
Wish you the best.

[flotus1]

Since I was able to help you I would really appreciate if you could take a few minutes to look at my problem:

http://www.cfd-online.com/Forums/fluent/104124-problems-radiation-discrete-ordinates-model.html

cheerio

[fshak92]

Hi

I set the udf to the boundary condition of the line(the line in the picture below) as 'heat flux' and 'temperature' ,but non of them changed any thing in my 'temperature contour' after running for some seconds.
The simulation is 3d but the coordinates of line is changing just in Y ,therefore i replaced all the 'X' , to 'Y'.
Is there any hint that should be considered?
Thank you again.

[flotus1]

The names of the Variables have nothing to do with the ordinates.
The array x[ND_ND] holds the position vector, but could easily be called position[ND_ND] or thisisabitconfusing[ND_ND]

x[0] -> x-position
x[1] -> y-position
x[2] -> z-position (if the case is 3D)

[hannarose]

Originally Posted by flotus1

If your boundary condition is just a heat flux, then set the BoCo to "wall" and apply a User Defined Function (UDF) as the thermal condition.
A UDF is a text file wit a .c extension which can be interpreted by fluent directly.

For a simplified 2-dimensional case with the laser beam moving in x-direction and having a rectangular intensity distribution, the UDF might look like this:

#include "udf.h"

DEFINE_PROFILE(laser_beam,t,i)                //Randbedingung für den Energiefluss durch den Laser
{
    real x[ND_ND];                   //Ortsvektor; ND liest aus ob 2D oder 3D-Fall
    real X;                             //Ortskoordinate
    real x_0=0.05;                   //starting point
    real v=0.05;                     //velocity of the laser beam
    real b=0.005;                    //width of the laser beam
    real I_0=50000000;            //Intensity
    real time=RP_Get_Real("flow-time");        //der Variable time wird die Simulationszeit zugewiesen
    face_t f;
    begin_f_loop(f,t)
    {
        F_CENTROID(x,f,t);            //liest Koordinate aus
        X=x[0];
        if(X>=x_0+time*v-b/2 && X<=x_0+time*v+b/2)    //Laser bewegt sich entlang X
            F_PROFILE(f,t,i) = I_0;
        else
            F_PROFILE(f,t,i) = 0;
    }
    end_f_loop(f,t);
}

Put the code in a text file, for example beam.c
In Fluent, go to "define" - "user defined" - "functions" - "interpreted" and choose the file. Click on "Interpret".
Now when setting up the heat flux for the boundary condition, the drop down menu which reads "constant" should allow picking the "laser_beam" profile defined in the UDF.

Since I want to simulate melting of the material by the laser, I am no longer using a heat flux as a boundary condition. Instead, I am trying to use the Discrete Ordinates radiation model to simulate the laser beam.
But if you just want to heat up the material, a heat flux BoCo should be sufficient.

hye. i will be doing a modeling of laser cutting. the parameters are cutting speed, laser power, focal length. how can i do the modeling using ansys? i want to get the thermal distribution and kerf width.tq

[flotus1]

http://www.cfd-online.com/Forums/flu...tes-model.html