# how to access second derivative of velocity

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

 December 7, 2005, 14:28 how to access second derivative of velocity #1 Lichun Dong Guest   Posts: n/a hi, all: Does anyone knows how to access second derivative of velocity in FLUENT (such like du2/d2x)? I am thinking about calculating it using first derivative (we can access it in FLUENT). But I can not get the value of a specific cell and its neighbor cell. Thanks very much lichun

 December 8, 2005, 04:26 Re: how to access second derivative of velocity #2 RoM Guest   Posts: n/a I have written an udf that claculates du/dx but i don think its 100% flawless. It uses equation 26.2-7 from the users guide. The calculated values for du/dx are always slightly different from the ones calculated by fluent so i guess the code needs some improvent or maybe fluents solver uses a different approach. You can alter the udf to calculate d2u/dx2 by replacing all C_U with C_DUDX. Good luck, RoM DEFINE_ON_DEMAND(calc_dudx) { Domain *d; Thread *ct,*ft; face_t f; cell_t c; int n; real A[ND_ND],c_cen[ND_ND],f_cen[ND_ND],c_f[ND_ND]; real dudx,u_mean,sign; d=Get_Domain(1); thread_loop_c(ct,d) { begin_c_loop(c,ct) { dudx=0.; C_CENTROID(c_cen,c,ct); c_face_loop(c,ct,n) { f=C_FACE(c,ct,n); ft=C_FACE_THREAD(c,ct,n); F_AREA(A,f,ft); F_CENTROID(f_cen,f,ft); NV_VV(c_f,=,f_cen,-,c_cen); if((NV_DOT(A,c_f)>0) sign = 1.; else sign -1.; if(BOUNDARY_FACE_THREAD_P(ft)) u_mean=C_U(c,ct); else u_mean=0.5*(C_U(F_C0(f,ft),THREAD_T0(ft))+C_U(F_C1 (f,ft),THREAD_T1(ft))); dudx+=(sign*u_mean*A[0]); } dudx/=C_VOLUME(c,ct); C_UDMI(c,ct,0)=dudx; } end_c_loop(c,ct) } }

 December 8, 2005, 04:34 Re: how to access second derivative of velocity #3 zxaar Guest   Posts: n/a fluent restricts these values of derivatives to use in the code, so they are multiplied by a factor alpha, calculated based on venkatakrishanans limiter. The derivatives that you have calculated are unbounded derivatives.

 December 8, 2005, 04:50 Re: how to access second derivative of velocity #4 RoM Guest   Posts: n/a In my case the calculated values where lower (about 10%) than the ones from fluent. Dou you have ideas why this happens? RoM

 December 8, 2005, 05:59 Re: how to access second derivative of velocity #5 zxaar Guest   Posts: n/a I am not sure what exactly happened, but fluents gradient process is bit different, i will outline them for you, [*] Calculate the gradients with face value taken as mean phi_f = 0.5 * (phi_0 + phi_1), as you have calculated[*] Restrict them, so that the face value calculated by them shall not exceed the local maxima minima, phi_f = phi_0 + grad . (delta r)[*] now calculate the face value as phi_f = 0.5 * (phi_f_0 + phi_f_1), where phi_f_0 = phi_0 + grad_0 . (delta r) and phi_f_1 = phi_1 + grad_1 . (delta r), now calculate the gradients again. So there will be difference between what you calculate then what fluent does, wise thing is to use them directly, since it will not make the solution blow up wond likes this.

 December 8, 2005, 06:34 Re: how to access second derivative of velocity #6 RoM Guest   Posts: n/a Thanks you very much for this explanation. I find the time i will try it out just to see if the difference between the udf and the fluent values will go away. Btw i had a typo in the source i posted above "if((NV_DOT(A,c_f)>0) sign = 1.; else sign -1.;" should be "if((NV_DOT(A,c_f)>0)) sign = 1.; else sign =-1.;" , just in case someone trys to compile this mess. Thanks again, RoM

 December 8, 2005, 12:09 Re: how to access second derivative of velocity #7 Lichun Dong Guest   Posts: n/a Thanks for your response. really appreciate. lichun

 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 Ozgur_ FLUENT 5 August 25, 2015 04:58 sarah_ron2002 FLUENT 5 December 20, 2006 11:44 Asghari FLUENT 1 October 23, 2006 06:23 Antech Main CFD Forum 0 April 25, 2006 02:15 chong chee nan FLUENT 0 December 29, 2001 06:13

All times are GMT -4. The time now is 13:01.