[mariam.sara]

Hello I have 3D channel flow I wrote a UDF for velocity profile at inlet to get fully developed flow I need to enter average velocity into my UDF as input parameter? How i can do this please? any help is mandatory?

mariam

[mariam.sara]

Nobody know my question?

mariam

[hwet]

Not sure but the way it sounds "average velocity", I would just use a velocity inlet condition, thats what i suppose it does? why do you even need a UDF for an average profile?

[pakk]

Are you asking us for help on the udf that you wrote? You are the creator, so you should know best how it works...
And anyway, how do you think we can tell you how your own udf works if you don't give us the code? We are not telepathic...

[mariam.sara]

Thanks hwet for the replay. I want use different Uavg values at the udf because I want set different velocities for inlets because I have heat exchanger of two fluids (water and air) contain several inlets for air (its number reach 100) hence I need 100 udf so I just want set Uavg as an input parameter in the udf and let it change inside the udf hope this clear??

Originally Posted by hwet

Not sure but the way it sounds "average velocity", I would just use a velocity inlet condition, thats what i suppose it does? why do you even need a UDF for an average profile?

[mariam.sara]

Mr. pakk my question not about the udf and if it working or no. My question about how i can using parameter in udf (see photo)? i need steps how to really applied a parameter to the udf?

Originally Posted by pakk

Are you asking us for help on the udf that you wrote? You are the creator, so you should know best how it works...
And anyway, how do you think we can tell you how your own udf works if you don't give us the code? We are not telepathic...

[mariam.sara]

Hi pakk to be more specific I have a UDF which requires a real parameter. Is there a way to give this parameter different values, without having to modify and recompile the udf again? if you want to have a look on the udf i will post it?

Originally Posted by pakk

Are you asking us for help on the udf that you wrote? You are the creator, so you should know best how it works...
And anyway, how do you think we can tell you how your own udf works if you don't give us the code? We are not telepathic...

[pakk]

Originally Posted by mariam.sara

Hi pakk to be more specific I have a UDF which requires a real parameter. Is there a way to give this parameter different values, without having to modify and recompile the udf again? if you want to have a look on the udf i will post it?

You can set a parameter in the text user interface. If you want to set a parameter with the name 'tui_alpha' to the value 0.05, type the following in Fluent:

(rp-var-define 'tui_alpha 0.05 'real #f)

To read this parameter into the c-code udf, you can use the following code in your udf:

udf_alpha = RP_Get_Float("tui_alpha");

For more help, look for "rp-var-define" and "RP_Get_Float" in the Fluent manual.

[mariam.sara]

Thanks pakk for the valuable answer. Actually I was followed the steps mentioned in user guide and I type the option for my average velocity as below in text interface:

rp-var-define 'Uavg 0.05' real #f

the problem when i compile my udf the following error appear to me:

Error: rpgetvar: Uave: undefined variable

what the problem? knowing i was added the variable in the UDF and here is copy of the full UDF

/************************************************** *******************
UDF for specifying steady-state velocity profile boundary condition
************************************************** ********************/
#include"udf.h"
/* Geometry description */
#define h 0.002 /*height duct in m */
#define w 0.005 /*weidth duct in m */
#define s 0.004 /*step weidth duct in m */
/*********** ****************************
Inlet velocity profile
***************************************/
DEFINE_PROFILE(inlet_z1_velocity,t,i)
{
real x,z1[ND_ND];
real radx,rady,;
real N1,M1,Alfa;
real y;
face_t f;
real Uave=RP_Get_Real("Uave");
Alfa =(w/h); /* Aspect ratio of the inlet duct */
M1 = 1.7 + 0.5 * pow(fabs(Alfa),-1.4);
if (Alfa <= (1/3))
N1 = 2.0 ;
else
{
N1 = 2 + 0.3*(Alfa - (1/3));
}
/*********************************************/
begin_f_loop(f,t)
{
F_CENTROID(z1,f,t);
y = z1[1];
x = z1[2];
rady = (1.0-pow(fabs(y-h/2)/(h/2),N1));
radx = (1.0-pow(fabs(x-((w/2)+ s))/(w/2),M1));
F_PROFILE(f,t,i) = Uave*((M1+1)/M1)*((N1+1)/N1)*rady*radx;
}
end_f_loop(f,t)
}

[ghost82]

rp-var-define 'Uavg 0.05' real #f

real Uave=RP_Get_Real("Uave");


Then it is not rp-var-define 'Uavg 0.05' real #f
but
rp-var-define 'Uavg 0.05 'real #f

[mariam.sara]

Thanks ghost for the reply. I not understand your replay clearly may you tell me what the error with my expression? It seem you wrote similar expression to the one I wrote?

mariam

Originally Posted by ghost82

rp-var-define 'Uavg 0.05' real #f

real Uave=RP_Get_Real("Uave");


Then it is not rp-var-define 'Uavg 0.05' real #f
but
rp-var-define 'Uavg 0.05 'real #f

[ghost82]

You defined Uavg as variable but you call Uave in udf, which is not defined. So, change Uavg to Uave

[mariam.sara]

I fixed this error but the current error shown in picture is still appearing to me as soon as i open fluent?? what its reason?

Originally Posted by ghost82

You defined Uavg as variable but you call Uave in udf, which is not defined. So, change Uavg to Uave

[ghost82]

Fluent cannot find the libudf folder with compiled udf to load it, nor the .c file to autocompile udf.
Do you have the libudf folder or the .c file in the same folder in which you have the .cas?

[mariam.sara]

Cannot find the libudf folder? may you tell me where i can find it please?

Originally Posted by ghost82

Fluent cannot find the libudf folder with compiled udf to load it, nor the .c file to autocompile udf.
Do you have the libudf folder or the .c file in the same folder in which you have the .cas?

[ghost82]

You start with the cas and .c files in some folder; when you compile the .c file fluent automatically creates the "libudf" folder inside the folder where you have .c and .cas files. Inside the libudf folder there are other folders and your compiled udf. If you don't have the libudf folder fluent searches for the .c file and if it finds it, it will try to automatically recompile the code, recreating the libudf folder.

[engrmansoor2534]

Can anyone please explain the purpose of the terms used in the following UDF

#include"udf.h"
DEFINE_GRID_MOTION(twist,domain,dt,time,dtime)
{
Thread *tf = DT_THREAD(dt);
face_t f;
Node *v;

real NV_VEC(axis);
real delta,xaxis,yaxis,teta,xn,yn,dx,dy,H;
int n;


H = 0.1; /*z-dimension of the model*/
teta = 10*3.14/180; /*rotation angle*/


begin_f_loop(f,tf)
{
f_node_loop(f,tf,n)
{
v = F_NODE(f,tf,n);
/* update node if the current node has not been previously
visited when looping through previous faces */
if ( NODE_POS_NEED_UPDATE (v))
{
/* indicate that node position has been update
so that it's not updated more than once */
NODE_POS_UPDATED(v);
xn = cos(teta)*NODE_X(v)-sin(teta)*NODE_Y(v);
yn = sin(teta)*NODE_X(v)+cos(teta)*NODE_Y(v);
dx = xn-NODE_X(v);
dy = yn-NODE_Y(v);
xaxis = dx/sqrt(pow(dx,2) + pow(dy,2));
yaxis = dy/sqrt(pow(dx,2) + pow(dy,2));
NV_D(axis, =, xaxis,yaxis, 0.0);
delta = sqrt(pow(dx,2) + pow(dy,2))*NODE_Z(v)/H;
NV_V_VS(NODE_COORD(v), =, NODE_COORD(v), +, axis,*,delta);


}
}
}
end_f_loop(f,tf);
}

this UDF produces a twist in a channel. I got it from one of cfd-online posts. I need to know the physical meaning of the lines in BOLD.
thank you

[brunoc]

It's math. Everything it does is written there, and the functions (NODE_X(), NODE_Y(), NV_D(), etc) are in the manual.

What don't you understand?