[Supernova]

Dear all,

I am trying to get some udfs for variable viscosity working in Fluent 6.3, although I'm having a great deal of problems in doing so...

I want to interpret the following code:

#include "udf.h"
//Works Casson
DEFINE_PROPERTY(cell_viscosity,c,t)
{
double mu_lam

double tiny = 0.0000000001;
double tauy = 0.01083;
double muinf = 0.0031;
double m = 200;
double strain;
double first;

strain = pow(C_DUDX(c, t),2)+ pow(C_DVDY(c, t),2)+
pow(C_DWDZ(c, t),2)+
2*pow(C_DUDY(c, t)+ C_DVDX(c, t),2)+
2*pow(C_DUDZ(c, t)+ C_DWDX(c, t),2)+
2*pow(C_DVDZ(c, t)+ C_DWDY(c, t),2);

strain = pow(strain, 0.5);

first = 1-exp(-pow(m*strain,0.5));

mu_lam = pow(muinf,0.5) + pow(tauy/(strain + tiny),0.5)*first;

mu_lam = pow(mu_lam, 2);
if(cell==100){printf("viscosity = %f",mu_lam);}
return mu_lam;
}


However, when I read my case file, and try to interpret this, I get the following error:

Error: c:\fluent.inc\fluent6.3.26/src/dpm.h: line 1192: parse error.

I would greatly appreciate any help I could get on this.

Many thanks in advance. Richard

[Supernova]

Can anyone please help me with this?

My final year project depends on this, and I don't know much about programming...

Thank you.

[Supernova]

Actually forget it, I figured it out in the end: I had my header file in the same folder as my code, so it didn't work!

[Jane]

Hi, Supernova

strain = pow(C_DUDX(c, t),2)+ pow(C_DVDY(c, t),2)+
pow(C_DWDZ(c, t),2)+
2*pow(C_DUDY(c, t)+ C_DVDX(c, t),2)+
2*pow(C_DUDZ(c, t)+ C_DWDX(c, t),2)+
2*pow(C_DVDZ(c, t)+ C_DWDY(c, t),2);


may i know how do you difine the C_DUDX (c,t) and the rest in your UDF??

[coglione]

hello Jane,

C_DUDX(c,t) is a predefined macro which returns the derivative of x-velocity with respect to x-coordinate. You do not have to define it by yourself. However there is also a macro C_STRAIN_RATE_MAG(c,t) to access the strain rate for each cell itself, thus there is no reason to compute this value by hand.

cheers

[Jane]

Hi, coglione

Thank you for your reply.

for example if i wan to code the equation as show in figure. below is the equation that i code for UDF.

shear_rate = sqrt (SQR(C_DUDX(c,t))+ SQR(C_DVDY(c,t) + SQR(C_DWDZ(c,t));

may i know the equation that i code into UDF is correct or not?

[Jane]

Originally Posted by Jane

Hi, coglione

Thank you for your reply.

for example if i wan to code the equation as show in figure. below is the equation that i code for UDF.

shear_rate = sqrt (SQR(C_DUDX(c,t))+ SQR(C_DVDY(c,t) + SQR(C_DWDZ(c,t));

may i know the equation that i code into UDF is correct or not?

Help me please...
i'm just a UDF beginner...please tell me

[coglione]

Hello Jane,

the correct equation for strain rate is given by supernova in the first message of this thread. Use his coding or simply the macro C_STRAIN_RATE_MAG(c,t). It will return excactly the same and is much more efficient in terms of cpu-time.

cheers

[Jane]

Originally Posted by coglione

Hello Jane,

the correct equation for strain rate is given by supernova in the first message of this thread. Use his coding or simply the macro C_STRAIN_RATE_MAG(c,t). It will return excactly the same and is much more efficient in terms of cpu-time.

cheers

Hi coglione,

thank you for your reply

i've tried macro C_STRAIN_RATE_MAG(c,t) in the UDF, the problem occurs when i simulate using this predefined strain rate. the continuity graph increase until fluent show errors message.

i suspect my shear rate equation caused the increase of continuity, but i still cannot find the solution.

can you give me some idea?

[coglione]

Hello Jane,
non-newtonian fluids are always prone for numerical problems due to the highly non-linear nature of the momentum equation involved. I usually start the simulation with a moderate shear dependency of the viscosity (or even constant one) and switch to the actual rheological model when the approximate solution has converged. This provides a realistic and quite smooth strain field and may help convergence. If instability is still observed lower your relaxation, use first order discretization and if nothing helps at all switch to transient simulation using a small time-step.

Hope this helps

[Jane]

Originally Posted by coglione

Hello Jane,
non-newtonian fluids are always prone for numerical problems due to the highly non-linear nature of the momentum equation involved. I usually start the simulation with a moderate shear dependency of the viscosity (or even constant one) and switch to the actual rheological model when the approximate solution has converged. This provides a realistic and quite smooth strain field and may help convergence. If instability is still observed lower your relaxation, use first order discretization and if nothing helps at all switch to transient simulation using a small time-step.

Hope this helps

Thank you for your advice, finally i get the stable continuity.
Thank you very much

I found my UDF unable to print the numbers to console.

Below is my "message" in UDF.

/*Message("UDF: time=%f,shear_rate=%f");*/

[Daniel Tanner]

Leave out the outer quotation marks.

"Message("UDF: time=%f,shear_rate=%f");"

should be of the form

Message("UDF: time=%f,shear_rate=%f", X, Y);

where X and Y are the time and shear_rate variables, i.e., you have not told the MESSAGE macro where to find the time and shear rate variables.

[Jane]

Originally Posted by Daniel Tanner

Leave out the outer quotation marks.

"Message("UDF: time=%f,shear_rate=%f");"

should be of the form

Message("UDF: time=%f,shear_rate=%f", X, Y);

where X and Y are the time and shear_rate variables, i.e., you have not told the MESSAGE macro where to find the time and shear rate variables.

Thank you very much

[maple]

Originally Posted by coglione

hello Jane,

C_DUDX(c,t) is a predefined macro which returns the derivative of x-velocity with respect to x-coordinate. You do not have to define it by yourself. However there is also a macro C_STRAIN_RATE_MAG(c,t) to access the strain rate for each cell itself, thus there is no reason to compute this value by hand.

cheers

Hi Coglione,

Your input here has been very useful in my project.
I would like to ask a few questions:

C_STRAIN_RATE_MAG(c,t) deos it give a dimensionless value? or just the strain rate?

This is me code for my model:
#include"udf.h"
DEFINE_PROPERTY(c_effective_viscosity, cell, thread)
{
double e_viscos;
double m = 200;
double a_viscos = 0.0031;
double y_stress = 0.01082;
double strain;
double a;
double b;
double c;
strain = C_STRAIN_RATE_MAG(cell,thread);
a = y_stress/strain;
b = m*strain;
c = 1-exp(-pow(b,0.5));
e_viscos = pow(a_viscos,0.5)+(pow(a,0.5)*c);
e_viscos = pow(e_viscos,2);
return e_viscos;
}

However, when I try to run it, Fluent does not start iterating and shows the following error message.
Error: Floating point error: invalid number
Error Object: ()

Can you please help?


Regards,
Maple

[wendywu]

Hello,
I am writing a nonNewtonian viscosity model of my own,
in the myViscosityModel.c, I wrote
shearrate=max(minshearrate, sqrt(2.0*(symm(fvc::grad(u)))&&(symm(fvc::grad(u)) )/3.0);

when I compile it with "wmake",
error is given as :
arguments in max()function has different dimensions
[0 0 -1 0 0 0 0] and [0 0 0 0 0 0 0],
then I tried to delete one argument, as:
shearrate= sqrt(2.0*(symm(fvc::grad(u)))&&(symm(fvc::grad(u)) )/3.0;
wmake it, still one error exist, but I didn't found out the error,
then I changed it back, as original:
shearrate=max(minshearrate, sqrt(2.0*(symm(fvc::grad(u)))&&(symm(fvc::grad(u)) )/3.0);
then I wmake it, still one error ,but this time the output is much more than the first time, I can not find where the error is,
I am confused, the same code, leads to different output, what is the problem?
I checked the dimensions of the two arguments of max(), there are both 1/second, why it thinks the second argument 's dimension is [0 0 0 0 0 0 0]?
anybody has any idea? thank you. and sorry for disturbing.

wendy

[coglione]

Are you sure this is the right forum for this question?
It sounds pretty much like OpenFoam which has its own userforum here on cfd-online.
cheers

[wendywu]

Originally Posted by coglione

Are you sure this is the right forum for this question?
It sounds pretty much like OpenFoam which has its own userforum here on cfd-online.
cheers

yeah, Thank you for reminding.

[m zahid]

hi, anybody know the difference between "strain rate" and "scale of strain rate".

please share your knowledge.
regards

[Abhijeeth]

Originally Posted by coglione

hello Jane,

C_DUDX(c,t) is a predefined macro which returns the derivative of x-velocity with respect to x-coordinate. You do not have to define it by yourself. However there is also a macro C_STRAIN_RATE_MAG(c,t) to access the strain rate for each cell itself, thus there is no reason to compute this value by hand.

cheers

Can this macro C_STRAIN_RATE_MAG(c,t) be used for Cylindrical coordinate system

[Abhijeeth]

Originally Posted by coglione

hello Jane,

C_DUDX(c,t) is a predefined macro which returns the derivative of x-velocity with respect to x-coordinate. You do not have to define it by yourself. However there is also a macro C_STRAIN_RATE_MAG(c,t) to access the strain rate for each cell itself, thus there is no reason to compute this value by hand.

cheers

Can this macro C_STRAIN_RATE_MAG(c,t) be used for Cylindrical coordinate system