[CaptainCombo]

Hi,
I am trying to define momentum source representing manteic field using UDF in Ansys Fluent. There will be one magnet placed above or below of the channel as it is shown in image. The problem is placing the magnet above and below of the channel cause compeletely different results. However since there is no gravity effect I was expecting these two cases should be symmetricay just like an image in mirror. Magnet position 2 gives compeletely irrevelant results.I would like to see contour plot of momentum source therefore maby I could be able to figure out the problem. Is there any way to plot momentum source.
Here is my UDF code;

#include "udf.h"
#include <math.h>       /* sin */

#define PI 3.14159265
#define a1 0.2 /* these are magnet coordinates */
#define b1 -0.5
#define a2 0.2
#define b2 0.5


DEFINE_SOURCE(B_x,c,t,dS,eqn)
{ 
  real source;
  real pos_x;
  real pos_y;
  real x[ND_ND];
  pos_x = x[0];
  pos_y = x[1];
  
	
  F_CENTROID(x, c, t);	
 
  source = 2*0.0000001*50*-1/sqrt(pow((pos_x-a1),2)+pow((pos_y-b1),2))*0.35*(pos_x-a1)/pow((pow((pos_x-a1),2)+pow((pos_y-b1),2)),1.5);
 
  dS[eqn] = 0;

  return source;
}

Also,I got this warning during compile udf is this may be related my problem?
udf_names.c(12) : warning C4113: 'void (*)()' differs in parameter lists from 'void (*)(void)'

[AlexanderZ]

that warning is normal

your source is dependent on pos_x pos_y that's why you have difference
when you apply it on top and bottom plates. (cause of different y values)

[CaptainCombo]

Originally Posted by AlexanderZ

that warning is normal

your source is dependent on pos_x pos_y that's why you have difference
when you apply it on top and bottom plates. (cause of different y values)

When I calculate the source in excel for same distances away from the magnet position 1 or 2 the equation gives same values regardless the pos_x and pos_y. pos_x and pos_y are epicenter of the source, and magnitude of the source is depend on the distance not the central position of it.

[pakk]

No, in your UDF, pos_x and pos_y is the position on which you should calculate the source.

Different pos_x and pos_y have different distances to the magnet,so different values.

[CaptainCombo]

Originally Posted by pakk

No, in your UDF, pos_x and pos_y is the position on which you should calculate the source.

Different pos_x and pos_y have different distances to the magnet,so different values.

Consider I am simulating magnet placed bottom of the channel, so central cooridnates of the soruce will be a1 and b1. Let's say magnetic source at pos_x = 0.2 and pos_y = -0.4 is calculated from the equation as M1. In second case I switched a1 with a2 and b1 with b2 therefore magnet will be placed at the top of the channel. Magnetic source at the same distance away from the new position which is pos_x = 0.2 and pos_y = 0.4 (distance is 0.1 in y-direction in both case) will be M2. When I calculate this in excel I get same value in both cases(M1 = M2). Same situation should be avaiable in simulation in fluent but positioning the magnet different locations gives compeletely different flow patterns.

[pakk]

Can you show the code that you used for magnet 2 (just to make sure that you replaced everything correctly) and a plot of the "irrelevant results" with magnet 2?

[pakk]

  pos_x = x[0];
  pos_y = x[1];
  F_CENTROID(x, c, t);

This should be given a warning when you compiled: you read the value of x before setting it!

Put the centroid line first. And I think you should use C_CENTROID, because you work with cells, not faces.

Are you really sure you compiled this code, and that there were no errors other than the names.c error?

[Yasser]

as Pakk mentioned, these two lines must go below the C_CENTROID line

pos_x = x[0];
pos_y = x[1];

[CaptainCombo]

Now it works friends. I have been struggling this for a few days since, it was compiled in each case I was not suspicious about the code. The flow pattern was not as I expected but at least I was hoping to get symetrical results. Now the flow pattern is as I expected and it is symetrical as shown pictures below.







If I know you in real life I would take you dinner tonight.



Thank you very much!

[kien]

Hi, could you share the code and please show me how to add the magnet in Ansys fluent,

I am new in Ansys Fluent, and I want to simulate the blood flow under magnetic field created by magnet,

Thank you

Originally Posted by CaptainCombo

Now it works friends. I have been struggling this for a few days since, it was compiled in each case I was not suspicious about the code. The flow pattern was not as I expected but at least I was hoping to get symetrical results. Now the flow pattern is as I expected and it is symetrical as shown pictures below.







If I know you in real life I would take you dinner tonight.



Thank you very much!