CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > STAR-CCM+

Moving Laser Beam

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree6Likes
  • 2 Post By fshak92
  • 1 Post By flotus1
  • 2 Post By flotus1
  • 1 Post By flotus1

Reply
 
LinkBack Thread Tools Display Modes
Old   June 18, 2012, 07:32
Default Moving Laser Beam
  #1
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
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.
fuguang and vishnumaya like this.

Last edited by fshak92; June 19, 2012 at 08:45.
fshak92 is offline   Reply With Quote

Old   June 25, 2012, 04:46
Default
  #2
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
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 is offline   Reply With Quote

Old   June 29, 2012, 05:02
Default
  #3
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
Nobody has any idea?
fshak92 is offline   Reply With Quote

Old   July 3, 2012, 04:07
Default
  #4
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,049
Rep Power: 18
flotus1 will become famous soon enoughflotus1 will become famous soon enough
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 likes this.

Last edited by flotus1; July 3, 2012 at 10:51.
flotus1 is offline   Reply With Quote

Old   July 3, 2012, 10:50
Default
  #5
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
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...
fshak92 is offline   Reply With Quote

Old   July 3, 2012, 11:09
Default
  #6
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,049
Rep Power: 18
flotus1 will become famous soon enoughflotus1 will become famous soon enough
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:

Code:
#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 and czhao86 like this.
flotus1 is offline   Reply With Quote

Old   July 3, 2012, 11:14
Default
  #7
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
Many Many Thanks to you indeed:-)
Wish you the best.
fshak92 is offline   Reply With Quote

Old   July 3, 2012, 12:00
Default
  #8
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,049
Rep Power: 18
flotus1 will become famous soon enoughflotus1 will become famous soon enough
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
flotus1 is offline   Reply With Quote

Old   July 25, 2012, 03:16
Default
  #9
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
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.
Attached Images
File Type: jpg laser-beam1.JPG (35.2 KB, 38 views)
fshak92 is offline   Reply With Quote

Old   July 25, 2012, 03:35
Default
  #10
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,049
Rep Power: 18
flotus1 will become famous soon enoughflotus1 will become famous soon enough
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)
fshak92 likes this.
flotus1 is offline   Reply With Quote

Old   December 11, 2012, 02:52
Default
  #11
New Member
 
hanna rose
Join Date: Dec 2012
Posts: 1
Rep Power: 0
hannarose is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
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:

Code:
#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
hannarose is offline   Reply With Quote

Old   December 11, 2012, 05:10
Default
  #12
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,049
Rep Power: 18
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Problems with radiation (discrete ordinates model)
flotus1 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
jagged, ragged edges... ziemowitzima OpenFOAM Native Meshers: snappyHexMesh and Others 138 July 23, 2012 23:41
HELP - Moving car simulation in fluent Brad Wells FLUENT 6 February 27, 2012 03:14
Moving mesh in Fluent fivos FLUENT 0 April 2, 2010 09:45
help on radiation model for a moving laser beam nazeem FLUENT 1 April 20, 2009 10:34
Effect of fire on a steel beam Amanda Fry FLUENT 1 January 20, 2004 14:59


All times are GMT -4. The time now is 23:43.