
[Sponsors] 
May 17, 2018, 23:37 
floating point exception

#1 
New Member
Join Date: May 2018
Posts: 5
Rep Power: 6 
Hi, everybody. I tryied to use a nonarrhenius 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 xvelocity yvelocity energy ch4 h2 co co2 time/iter Stabilizing species0 to enhance linear solver robustness. Divergence detected in AMG solver: species0 Stabilizing species1 to enhance linear solver robustness. Divergence detected in AMG solver: species1 Stabilizing species2 to enhance linear solver robustness. Divergence detected in AMG solver: species2 Stabilizing species3 to enhance linear solver robustness. Divergence detected in AMG solver: species3 Stabilizing temperature to enhance linear solver robustness. Divergence detected in AMG solver: temperature WARNING: Invalid cp (0.000000e+00 J/kgK) for mixturetemplate 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 /Tc4.063); K3 = K1 * K2; KCH4 = 6.65e6*exp(4604.28 / Tc); KH2O = 1.77e+3*exp(10666.35 / Tc); KH2 = 6.12e11*exp(9971.13 / Tc); KCO = 8.23e7*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; } 

May 21, 2018, 09:51 

#2 
Senior Member
Join Date: Sep 2017
Posts: 232
Rep Power: 10 
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); 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/gcc4...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 */ I advise you to crosscheck 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, "reaction1"))" 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 

May 21, 2018, 22:20 

#3  
New Member
Join Date: May 2018
Posts: 5
Rep Power: 6 
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:


March 9, 2021, 20:52 

#4 
New Member
Azharuddin
Join Date: Jan 2010
Posts: 4
Rep Power: 15 
Hello??
Any update on your issue??? I see similar errors when I compile my udf. Let me know. Thanks in advance. regards, 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
icoFoam floating point exception (8)  leizhao512  OpenFOAM Running, Solving & CFD  7  November 1, 2018 12:43 
A floating point exception has occurred: floating point exception [Overflow].  starlight  STARCCM+  4  May 4, 2016 10:08 
A floating point exception  SEM Model  yansheng  STARCCM+  1  April 4, 2016 05:57 
Floating point exception from twoPhaseEulerFoam  openfoammaofnepo  OpenFOAM Running, Solving & CFD  1  March 19, 2016 14:56 
Floating point exception (core dumped) for GAMG solver  yuhou1989  OpenFOAM Running, Solving & CFD  2  March 24, 2015 20:28 