CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT > Fluent UDF and Scheme Programming

floating point exception

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 17, 2018, 22:37
Unhappy floating point exception
  #1
New Member
 
Join Date: May 2018
Posts: 5
Rep Power: 6
ctmagic is on a distinguished road
Hi, everybody. I tryied to use a non-arrhenius reaction rate in my CFD model.
There are three reactions:
CH4+H2O=3H2+CO
CO+H2O= H2+CO2
CH4+2H2O=4H2+CO2

But I always get the Error reports as below. Could anyone tell me where is the problem?My UDF is also attached.

BTW: How to get the spieces ID? Is the spieces order in material mixture?

Detailed Error Info:
/************************************************** ******/
iter continuity x-velocity y-velocity energy ch4 h2 co co2 time/iter
Stabilizing species-0 to enhance linear solver robustness.

Divergence detected in AMG solver: species-0 Stabilizing species-1 to enhance linear solver robustness.

Divergence detected in AMG solver: species-1 Stabilizing species-2 to enhance linear solver robustness.

Divergence detected in AMG solver: species-2 Stabilizing species-3 to enhance linear solver robustness.

Divergence detected in AMG solver: species-3 Stabilizing temperature to enhance linear solver robustness.

Divergence detected in AMG solver: temperature

WARNING: Invalid cp (0.000000e+00 J/kgK) for mixture-template at temperature -1.#IND00 K


Warning: Mass_Diffusivity: invalid (zero) diffusivity.
Please check material properties.

Error at host: floating point exception

Error at Node 0: floating point exception

Error: floating point exception
Error Object: #f
************************************************** *********/
My UDF
/************************************************/
#include "udf.h"
#include "math.h"
#include "materials.h"
#define CH4 0
#define H2 1
#define CO 2
#define CO2 3
#define H2O 4
#define R_const 8.314
#define cata_density 2355.2
#define cata_porosity 0.51

DEFINE_VR_RATE(reforming_rate,c,t,r,mw,yi,rr,rr_t)
{
double k1, k2, k3, K1, K2, K3,KCH4,KH2,KCO,KH2O;
double Tc = C_T(c,t);
double gas_density = C_R(c,t);
double pCH4,pH2,pCO,pCO2,pH2O;
double DEN;
double r1m,r2m,r3m,r1v,r2v,r3v;
k1 = 9.49e+16*exp(-28879/Tc);
k2 = 4.39e+4*exp(-8074.3/Tc);
k3 = 2.29e+16*exp(-29336.0/Tc);
K1 = 10266.76*exp(-26830 /Tc+30.11);
K2 = exp(4400 /Tc-4.063);
K3 = K1 * K2;
KCH4 = 6.65e-6*exp(4604.28 / Tc);
KH2O = 1.77e+3*exp(-10666.35 / Tc);
KH2 = 6.12e-11*exp(9971.13 / Tc);
KCO = 8.23e-7*exp(8497.71 / Tc);


pCH4=(yi[CH4]*gas_density*R_const*Tc)/(mw[CH4]*1000);
pH2 = (yi[H2]*gas_density*R_const*Tc)/(mw[H2]*1000) ;
pCO = (yi[CO]*gas_density*R_const*Tc)/(mw[CO]*1000) ;
pCO2 = (yi[CO2]*gas_density*R_const*Tc)/(mw[CO2]*1000);
pH2O = (yi[H2O] * gas_density *R_const*Tc) / (mw[H2O]*1000);

DEN = 1 + KCO * pCO + KH2 * pH2 + KCH4 * pCH4 + (KH2O * pH2O / pH2);


r1m = 1000*k1 * (pCH4*pH2O - pow(pH2, 3)*pCO / K1) / (3600*pow(pH2, 2.5)*pow(DEN, 2));
r2m = 1000*k2 * (pCO*pH2O - (pH2*pCO2 / K2)) / (3600*pH2*pow(DEN, 2));
r3m = 1000*k3 * (pCH4*pow(pH2O, 2) - (pow(pH2, 4)*pCO2 / K3)) / (3600*pow(pH2, 3.5)*pow(DEN, 2));
r1v = r1m * cata_density*(1 - cata_porosity);
r2v = r2m * cata_density*(1 - cata_porosity);
r3v = r3m * cata_density*(1 - cata_porosity);

*rr=r1v;

}
ctmagic is offline   Reply With Quote

Old   May 21, 2018, 08:51
Default
  #2
Senior Member
 
Join Date: Sep 2017
Posts: 231
Rep Power: 9
obscureed is on a distinguished road
Hi ctmagic,

It is possibly worth paying attention to the error/warning messages about specific heat capacity and diffusivity -- although temperature may have diverged by the time those messages were generated.

I think it is essential to check that your UDF generates correct values. Apart from looking at the results and seeing that they are more or less reasonable, there are no checks apart from the ones you do yourself. So, as a debugging stage, print out every single value in the calculations -- but only for a few cells, or you will be swamped. The cell index, c, is really just an integer, so you can use something like:
Code:
if(c % 100000 == 37) Message("cell=%8d: Tc=%16.8g, DEN=%16.8g\n",c,Tc,DEN);
You might need to vary 100000 according to your model size; 37 is just an arbitrary low integer, and you could vary it to find an interesting or typical cell.

Since you want to print out more or less every variable in the UDF, you could try a "stringification" macro, as in https://gcc.gnu.org/onlinedocs/gcc-4...ification.html. Something like this (but I have not tried it exactly myself):
Code:
#define PRINTVAR(varname) do{ \
   if(c % 100000 == 37) \
    Message("cell=%8d: Tc=%16.8g, " #varname "=%16.8g\n" \
    ,c,Tc,varname); \
  } while(0)
PRINTVAR(k1);
PRINTVAR(k2);
/* etc etc etc */
See also https://gcc.gnu.org/onlinedocs/cpp/S...Semicolon.html

I advise you to cross-check some values in complete detail, by comparison with a spreadsheet or something. You might find, for example, that you have messed up the factor of 1000 when dealing with R/MW[i]. (To be honest, I think you probably have, though I am not sure. Fluent sticks closely to SI units, and the engineering way to accept molecular masses like C=12.0107 etc is to regard them as having units [kg/kmol]. Once you accept [kmol], then UNIVERSAL_GAS_CONSTANT is 8314.34, and it is #define'd as such in materials.h. But it is not safe to twiddle factors of 1000 until the results converge and look OK -- the point is that you need to check the whole thing. It is very easy to type "k1" instead of "K1", for example.) Even after you have checked that you hand over a rate in the correct units -- [kmol/(m3.s)] -- then you might like to check that Fluent is doing its part correctly in a test case.

You might find that the UDF is sometimes called with Tc==0., at least if you run from an initialized start. This is clearly crazy, and Tc is later initialized, but in general it is a good idea to make UDFs robust to crazy inputs -- even just returning all zeros.

By the way, I really like your "#define CH4 0" etc.

I presume you have only one equation, or else you would need to use the clunky tests "if (!strcmp(r->name, "reaction-1"))" etc, as in the help files.

It seems odd that you send back the result in *rr but not *rr_t -- I think this would be correct only for a laminar simulation (which is possible, I suppose).

Good luck!
Ed
obscureed is offline   Reply With Quote

Old   May 21, 2018, 21:20
Default
  #3
New Member
 
Join Date: May 2018
Posts: 5
Rep Power: 6
ctmagic is on a distinguished road
Hi, obscureed!
Many thanks for your patient reply,it's really helpful! I'll try to debug the UDF according to your suggestion.
Thanks again!

Quote:
Originally Posted by obscureed View Post
Hi ctmagic,

It is possibly worth paying attention to the error/warning messages about specific heat capacity and diffusivity -- although temperature may have diverged by the time those messages were generated.

I think it is essential to check that your UDF generates correct values. Apart from looking at the results and seeing that they are more or less reasonable, there are no checks apart from the ones you do yourself. So, as a debugging stage, print out every single value in the calculations -- but only for a few cells, or you will be swamped. The cell index, c, is really just an integer, so you can use something like:
Code:
if(c % 100000 == 37) Message("cell=%8d: Tc=%16.8g, DEN=%16.8g\n",c,Tc,DEN);
You might need to vary 100000 according to your model size; 37 is just an arbitrary low integer, and you could vary it to find an interesting or typical cell.

Since you want to print out more or less every variable in the UDF, you could try a "stringification" macro, as in https://gcc.gnu.org/onlinedocs/gcc-4...ification.html. Something like this (but I have not tried it exactly myself):
Code:
#define PRINTVAR(varname) do{ \
   if(c % 100000 == 37) \
    Message("cell=%8d: Tc=%16.8g, " #varname "=%16.8g\n" \
    ,c,Tc,varname); \
  } while(0)
PRINTVAR(k1);
PRINTVAR(k2);
/* etc etc etc */
See also https://gcc.gnu.org/onlinedocs/cpp/S...Semicolon.html

I advise you to cross-check some values in complete detail, by comparison with a spreadsheet or something. You might find, for example, that you have messed up the factor of 1000 when dealing with R/MW[i]. (To be honest, I think you probably have, though I am not sure. Fluent sticks closely to SI units, and the engineering way to accept molecular masses like C=12.0107 etc is to regard them as having units [kg/kmol]. Once you accept [kmol], then UNIVERSAL_GAS_CONSTANT is 8314.34, and it is #define'd as such in materials.h. But it is not safe to twiddle factors of 1000 until the results converge and look OK -- the point is that you need to check the whole thing. It is very easy to type "k1" instead of "K1", for example.) Even after you have checked that you hand over a rate in the correct units -- [kmol/(m3.s)] -- then you might like to check that Fluent is doing its part correctly in a test case.

You might find that the UDF is sometimes called with Tc==0., at least if you run from an initialized start. This is clearly crazy, and Tc is later initialized, but in general it is a good idea to make UDFs robust to crazy inputs -- even just returning all zeros.

By the way, I really like your "#define CH4 0" etc.

I presume you have only one equation, or else you would need to use the clunky tests "if (!strcmp(r->name, "reaction-1"))" etc, as in the help files.

It seems odd that you send back the result in *rr but not *rr_t -- I think this would be correct only for a laminar simulation (which is possible, I suppose).

Good luck!
Ed
ctmagic is offline   Reply With Quote

Old   March 9, 2021, 19:52
Default
  #4
New Member
 
Azharuddin
Join Date: Jan 2010
Posts: 4
Rep Power: 14
azharuddin0613 is on a distinguished road
Hello??

Any update on your issue???

I see similar errors when I compile my udf.

Let me know.

Thanks in advance.

regards,
azharuddin0613 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
icoFoam floating point exception (8) leizhao512 OpenFOAM Running, Solving & CFD 7 November 1, 2018 11:43
A floating point exception has occurred: floating point exception [Overflow]. starlight STAR-CCM+ 4 May 4, 2016 09:08
A floating point exception - SEM Model yansheng STAR-CCM+ 1 April 4, 2016 04:57
Floating point exception from twoPhaseEulerFoam openfoammaofnepo OpenFOAM Running, Solving & CFD 1 March 19, 2016 13:56
Floating point exception (core dumped) for GAMG solver yuhou1989 OpenFOAM Running, Solving & CFD 2 March 24, 2015 19:28


All times are GMT -4. The time now is 04:18.