BUG cavitation UDF

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 November 3, 2014, 12:19 BUG cavitation UDF #1 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 918 Rep Power: 15 ---------------- Last edited by ghost82; November 18, 2014 at 09:01.

 November 5, 2014, 10:48 #2 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 918 Rep Power: 15 It seems there's something more then this...I cannot compare results with the built in Schnerr and Sauer model with a custom udf in which is coded the same model. Results are completely different I tried both vofV=mafV[c] and vofV=mafV[c]*C_R(c,t)/rhoV[c] but no luck... This is udf: Code: ```#include "udf.h" DEFINE_CAVITATION_RATE(custom_cav, c, t, p, rhoV, rhoL, mafV, p_v, cigma, f_gas, m_dot) { real p_vapor = *p_v; real n_bubbles = 1.e12; real dp, Rb, vofV, source; dp = p_vapor-ABS_P(p[c],op_pres); vofV = mafV[c]; /* by printing on the console mafV is volume fraction not the mass fraction, probably a fluent bug */ Rb=pow((3.0*vofV/((1.-vofV)*4.0*M_PI*n_bubbles)), 1./3.); if (dp > 0.0) { source = sqrt(2/3*fabs(dp)/rhoL[c]); } else { source = -sqrt(2/3*fabs(dp)/rhoL[c]); } *m_dot = rhoV[c]*rhoL[c]/C_R(c,t)*3.*vofV*(1.-vofV)/Rb*source; }``` Equations are here: http://www.arc.vt.edu/ansys_help/flu...avitation.html Can anybody confirm if there is a bug or something else?

 November 6, 2014, 09:28 #3 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 918 Rep Power: 15 I wrote to ansys support..let's see what they say.. __________________ Google is your friend and the same for the search button! Last edited by ghost82; November 6, 2014 at 14:12.

 November 13, 2014, 10:42 #4 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 918 Rep Power: 15 Ok, this is the update from Ansys support, and I agree with their comments: 1-mafV in udf is vapor mass fraction 2-in the initialization panel the vapor fraction is mass fraction for Singhal et al cavitation model and volume fraction for the other models; so for custom cavitation udf the initialization panel requests mass fraction 3-in fluent post-processing when you plot vapor volume fraction, vapor volume fraction is plotted for every cavitation model My error was to consider in the initialization panel always vapor volume fraction. So, fluent (solver and post processing) is ok, however, it seems the bug is in cfd-post; I will update this thread if confirmed. __________________ Google is your friend and the same for the search button!

 November 18, 2014, 08:48 #5 Senior Member     Daniele Join Date: Oct 2010 Location: Italy Posts: 918 Rep Power: 15 Ok, this is solution to questions, thanks to Ansys support! 1- It is confirmed the bug in CFD-POST 15.0.7: if you define a custom cavitation udf (and maybe when using the Singhal et al cavitation model), save the cas and dat files in fluent, open CFD-POST and load the dat file, if you plot the vapor volume fraction variable it is plotted the vapor mass fraction. However, if you export from fluent the vapor volume fraction variable and you open the exported files (ascii or binary) in CFD-POST the plotted vapor volume fraction is correct. A request to solve the bug was posted. 2- Another problem I had is that if you define in udf the vapor volume fraction as: vofV = 1./(1.+(rhoV[c]/rhoL[c])*(1./mafV[c]-1.)) and you copy vofV values into C_UDMI: C_UDMI(c,t,0) = vofV if you plot in fluent cell centered values of C_UDMI(c,t,0) and vapor volume fraction values are different: this is because when you define a custom cavitation mass rate you have to turn on the Singhal et al cavitation model; this model takes into account also the incondensable mass fraction; if it is not zero when you plot the vapor volume fraction in fluent you are plotting secondary phase volume fraction (in my case steam+incondensable, and not only the steam volume fraction). If incondensable mass fraction is zero C_UDMI and vapor volume fraction values are the same. pakk likes this. __________________ Google is your friend and the same for the search button! Last edited by ghost82; November 18, 2014 at 11:07.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post kim FLUENT 3 October 26, 2011 21:38 AndresC FLUENT 0 February 25, 2010 16:50 Qureshi FLUENT 1 December 2, 2009 01:27 Puneet FLUENT 3 November 28, 2003 11:55 ROOZBEH FLUENT 4 May 29, 2003 09:54

All times are GMT -4. The time now is 00:07.

 Contact Us - CFD Online - Top