
[Sponsors] 
February 11, 2009, 05:37 
hi Hrv:
i am back.and here

#21 
Senior Member

Sponsored Links
i am back.and here is max residual plot of CFX and the interation procedure plot of total pressure difference of the inlet and outlet 

Sponsored Links 
February 11, 2009, 08:30 
hi Hrv:
i am back.and here

#22 
Senior Member

hi Hrv:
i am back.and here is max residual plot of CFX and the interation procedure plot of total pressure difference of the inlet and outlet regards wayne 

February 11, 2009, 08:54 
Hi Dragos:
the absolute vel

#23 
Senior Member

Hi Dragos:
the absolute velocity is below.would you mind tell me more? regardz! wayne 

February 11, 2009, 10:01 
Ok, the velocity looks physica

#24 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 649
Rep Power: 13 
Ok, the velocity looks physical as it looked in the relative values.
My guess now goes the same direction as Hrv said before: the results are not converged. Dragos 

February 11, 2009, 10:29 
Hi
do you mean both CFX a

#25 
Senior Member

Hi
do you mean both CFX and OF result are not converged?how about the max residual of CFX? how to determine if the result is converged? can you give me some example residual plot of converged ?? wayne 

February 11, 2009, 10:40 
hi
i also show the interat

#26 
Senior Member

hi
i also show the interation procedure plot of total pressure difference of the inlet and outlet, how about that? wayne 

February 11, 2009, 11:38 
here is the clear view of resi

#27 
Senior Member

here is the clear view of residual of OF result


February 12, 2009, 08:43 
How about my max residual plot

#28 
Senior Member

How about my max residual plot,and moniter pointing plot of CFX? and how about OF?
ara they all not converged? Regards wayne 

February 18, 2009, 08:27 
Hi wayne,
the CFX help tell

#29 
Member
Marco Müller
Join Date: Mar 2009
Location: Germany
Posts: 94
Rep Power: 10 
Hi wayne,
the CFX help tells: > 5e4 for MAX Residuals means: very poor, global balances will be poor and quantitative data is largely unreliable. This is good enough for getting a rough idea of flow phenomena or making pretty pictures ;) Did you run with double precision? Try this. MAX Residuals below 1e3 is nearly impossible if you have some bad "elements" in your mesh... (Your RMS values look OK..) Regards Marco 

February 18, 2009, 23:24 
Hi Marco
thanks,but how abo

#30 
Senior Member

Hi Marco
thanks,but how about my OpenFOAM Residual plot? why residual of p is so large.and u,v,w is just smalller than 1e3.you see i run OF in double precision but not of CFX. btw ,where did you find that " the CFX help tells: > 5e4 for MAX Residuals means: very poor, ".i have check for the help.but do not find it. thanks wayne 

February 19, 2009, 02:51 
Hi Wayne,
the topic I found

#31 
Member
Marco Müller
Join Date: Mar 2009
Location: Germany
Posts: 94
Rep Power: 10 
Hi Wayne,
the topic I found it is called "Judging Convergence" if I remember rightly... I have no experience in OF solving, I'm struggeling with mesh generation so far... ;) Marco 

February 19, 2009, 07:42 
Hi Wayne,
well, the thing a

#32 
New Member
olivier braun
Join Date: Mar 2009
Location: Lausanne, Switzerland
Posts: 19
Rep Power: 10 
Hi Wayne,
well, the thing about convergence is that you cannot expect any solver to yield a timeindependent solution on such a problem. We are talking about 25% of BEP flow rate, so massive flow separation will obviously occur and the fact that one of every two channels is stalled does not surprise me much. I know that in CFX you can easily monitor the torque you are looking for, might be interesting to know if this integrated quantity is fluctuating together with the high residuals. Olivier 

March 1, 2009, 07:51 
Hi Oliver and everyone
i

#33 
Senior Member

Hi Oliver and everyone
in the 25%BEP, there will be flow separation filled in passages.so it is hard to get a good result from timeindependent solver.i just want to know ,what level will steady solver in CFX and OF will achieve,if there will be jobs could do to make improvement,and what i want to do now is using OF result to compare with CFX result.but it is bad news that both get a pool level convergence.as you can see before. But it is for SST not for standard ke with scalable wall function in CFX,and in standard ke i will get smaller residual.that is smaller then 5e7(RMS) and 3e4(max),according to the CFX help it is good enough for engineering application.and the large residual is from the flow separation, and it could see as the error of turbulence model,not numerical tech.in other words,in my opinion,from the point of residual,the numerical error in CFX ke model is relative small for my case,and the errors should be from the modeling error,that say the error was from ke model. So i turn to SST,for i want more accurate boundary force or moment calculation.Then i got a worse convergence then standard ke in CFX,even worse in OF(seems).but both could get a pretty picture of follow pattern.and agree with the PIV result in reference paper.but the difference in definition of residual in CFX and OF let me don`t know if CFX and OF get a result in a similar accurate in numerical.and if the numerical level could not be considered compared with modeling error,and how i can i improve my result with SST in CFX and OF. The other thing is, starting with ke result i do a LES simulation(it get a convergence in smaller then 1e5 of RMS.poor values in separation area). SST in CFX get intergrate quantity between LES and standard ke,(for example if ke get moment coefficency number is 50%.then LES is 90％，and SST is 75%,the bad news is that OF get 45%..) so i want to know if the error is from numerical or from turbulence model. i wish it is from numerical.and i wish if the convergence will get the same level for SST in both CFX and OF similar to ke.so i could compared both of all. i wish some one could give me some good ideas wayne 

March 1, 2009, 09:05 
and here is integrated quanti

#34 
Senior Member

and here is integrated quantity iteration plot


March 1, 2009, 12:11 
and here is integrated quantit

#35 
Senior Member

and here is integrated quantity iteration plot


March 2, 2009, 03:40 
there must be something wrong

#36 
Senior Member

there must be something wrong with internet service here in hour school.
i will try again 

March 2, 2009, 04:04 
Hi Wayne,
maybe you can try

#37 
Member
Marco Müller
Join Date: Mar 2009
Location: Germany
Posts: 94
Rep Power: 10 
Hi Wayne,
maybe you can try to visualize the residuals in CFXPost by Isovolumes. (Writing residuals to .resfile has to be enabled in output settings before solving) If they are locally bad you can refine mesh there to ensure that you have no numerical errors... Marco 

March 2, 2009, 07:07 
Hi Marco
thanks!
i will try

#38 
Senior Member

Hi Marco
thanks! i will try as soon as possible and here is torque plot in OF iteration http://4ovewq.bay.livefilestore.com/y1paU9IyqdeXOCZ8_vychQT3ZQVdDsEV4hXiHoeGd4gv i_qGsxzzfjV5KZAfto1X5_CSeu2sQW8d8PLStQp8q_5WQ/Screenshot1.png here is torque plot in CF iteration http://4ovewq.bay.livefilestore.com/y1p_5WFzeMOsw5DUi59pUP_2u8AhtcrIaJDF4lSodkhl UbwTUqKkfLt_6ANDKoAU56OrBV6Q8Y8LWnchDVlMx6CLg/SST_moment.png wayne 

March 2, 2009, 09:48 
Hi Marco
i get the isovolumes

#39 
Senior Member

Hi Marco
i get the isovolumes of P mass residual with setting value =1e8,you could find picture here: http://4ovewq.bay.livefilestore.com/y1pZW9xQu2Vbt6gUbIJn5pIqSEfyPn26hG4x2zP7x_g2 sWQft_PahbDhRVlIyaTxh7wZMK8FFeeAyk/PmassRes.png isovolumes of U/V/W mass residual with setting value =1e6,you could find picture here: U: http://4ovewq.bay.livefilestore.com/y1pZW9xQu2Vbt6gUbIJn5pIqSEfyPn26hG4x2zP7x_g2 sWQft_PahbDhRVlIyaTxh7wZMK8FFeeAyk/PmassRes.png v: http://4ovewq.bay.livefilestore.com/y1pPRjqG4JN9m3T3SZYsL38KoXBrXxj_PkOFtc3NRNN o1UevzoY8Qf2nBkGhJMCF8UStbtdplo_rw/VmassRes.png W: http://4ovewq.bay.livefilestore.com/y1p12QArkUl1EJKaaFX9hGqTgy136YejAjDBwT9OlqxP aj_VOPQfqQARy3jZGcaFqSFx75G7xWbZnw/WmassRes.png How about the result?? do you think it is good enough for engineer application of torque calculation?? in my opinion ,in the blade domain the P/U/V/W residual is small enough, so the torque at blade is nothing wrong.but at Hub the U/V/W may get a relative coarse value so the viscous torque at Hub may not quiet precise,for pressure torque at Hub is zero.as the viscous torque is relative small compared with total torque.the total value of torque is with very small numerical error ,and the conclusion may be made as following: the error between this CFD result and real one is because of modeling error such as turbulent model.is that right? Regards wayne 

March 5, 2009, 13:57 
Hi Wayne,
in my opinion und

#40 
New Member
olivier braun
Join Date: Mar 2009
Location: Lausanne, Switzerland
Posts: 19
Rep Power: 10 
Hi Wayne,
in my opinion under these severe partial discharge conditions, it is neither the numerics, neither the choice amongst different flavours of RANS models that induce the most severe uncertainty but the general assumption of steadiness regarding simulation approach and boundary conditions. Did you use constant pressure outlet, or massFlow specified outlet? What was the experimental setup, what is the real one of engineering interest ? Impeller in infinite domain, I don't think so. At such conditions, all kind of stall in the impeller and diffuser can occur, the interaction with the tongue of a spiral casing / diffuser blades can induce torque and blade load peaks far beyond the average value that are more critical to the pump design than the steady value. Inlet recirculation far upstream of the impeller leading edges has been observed, can your b.c. take this into account. I went to time dependent RANS for some simulations done during my phD and had to find this is not sufficient. Just have to wait for another few decades and we can go DES for the entire beast over hundreds of impeller revolutions to do meaningful statistical averages of the flow in these washing machines ... Honestly, if I had to build a pump and needed to determine the torque at shutoff, I would rather believe in semiempirical statistic1D consideration mixes as published in pump design textbooks than in a timeindependent CFD simulation of an impeller without volute/diffuser... Cheers Olivier 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
analysis of pump flow in ANSYS  prakash  CFX  3  September 10, 2008 06:13 
ANSYS GMSH OpenFOAM  gtg627e  Open Source Meshers: Gmsh, Netgen, CGNS, ...  3  December 21, 2007 04:41 
turbulence model for water pump  Marcio  Main CFD Forum  4  September 3, 2003 09:35 
Water Pump to 10 year old kid  Selina Tracy  Main CFD Forum  1  February 11, 2003 23:19 
CFD Package for Water Pump Design !!!  John Sheng  Main CFD Forum  7  September 4, 2001 09:29 
Sponsored Links 