
[Sponsors] 
September 10, 2015, 07:12 
SIMPLE BCs for flow in parallel plates

#1 
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 
Hi,
I've recently coded up in C++ the SIMPLE algorithm for incompressible flow btn parallel plates (umomentum eq'n and mass eq'n). I'm using a staggered grid and following the book by Versteeg and Malalasekera (2007). I've run a few test cases with different BC's:  inlet velocity (uniform) with pressure outlet (0) > uniform velocity distribution throughout flow is attained.  inlet velocity (parabolic) with pressure outlet (0) > parabolic velocity distribution throughout flow is attained. Other BCs are u=0 at top and bottom wall (umomentum eq'n) and p'=0 for outlet. The pressure correction equation for top and bottom wall give p'=0 since the source term is always zero (u=0). And the pressure at the inlet is obtained by linear interpolation from inside the domain (Ferziger & Peric, 1997) My question is on the first case  is it correct? Isn't the flow supposed to develop into a parabolic profile towards the outlet? 

September 10, 2015, 07:28 

#2  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 
Quote:
yes, provided that the lengh of the plate is sufficient, you should get a parobolic velocity profile. What Re number do you set? 

September 10, 2015, 07:49 

#3 
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 

September 10, 2015, 08:15 

#4 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 
at such a Re number you cannot see a developed viscous profile........you have to reduce the Re number of some order of magnutude


September 10, 2015, 09:03 

#5 
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 

September 10, 2015, 09:28 

#6 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 

September 10, 2015, 10:25 

#7 
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 
I still obtain a uniform velocity profile.
the predicted velocity profile is okay but once i solve the pressure correction equation and correct the velocity, i obtain a uniform profile. See the attached matlab .fig files 

September 10, 2015, 11:01 

#8  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 
Quote:
At Re=1 you should see the viscous parablic profile...something is wrong...are you sure to have reached the steady state? 

September 10, 2015, 11:38 

#9  
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 
Quote:
Yes. At 200 iterations, only the predicted velocity changes but the corrected velocity is maintained. See attached. 

September 10, 2015, 11:46 

#10 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 
please, post directly the image... however, there is for sure something wrong in the code...check the BC.s after the correction, are they noslip conditions?


September 11, 2015, 07:55 

#11 
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 

September 11, 2015, 08:01 

#12 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 
you have a bug in the code ... at Re=1 you should see the two spatially evolving boundary layers


September 15, 2015, 14:43 

#13 
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 
After much debugging, i have some limited success  see images attached.
I get a more or less triangular profile near the outlet Ignore the pressure at inlet as I've not implemented the linear interpolation from inside the domain. 

September 15, 2015, 15:04 

#14 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 
you found the bug, the results seems physically reasonable now...you can compare with the analytical Blasius solution for a flat plane...then check that after some height a fully parabolic velocity profile is obtained
Of course, x=0 is a singular point. 

September 15, 2015, 15:27 

#15 
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 
My current issue is that it seems to develop a parabolic profile after entry but towards the outlet a "triangular" profile is acquired.


September 15, 2015, 16:06 

#16 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 
plot the velcoity at some station and superimpose the parabolic law...anyway, do you have ensured to have a suffient lenght do let the flow develop?


September 21, 2015, 05:33 

#17 
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 
Hopefully final question:
The momentum equations are linearized by using velocity and pressure fields from the previous outer iteration to solve for new fields. Now, at the end of an outer iteration, one has the new corrected velocity and pressure fields  u^{n},v^{n},p^{n}. Are residuals calculated based on the linearized momentum equations (ie using the old velocity fields to compute coefficients and old pressure field to compute flux and then apply the new velocity field to complete the equation) or are the residuals based on the nonlinear momentum equations (ie use the new velocity fields to compute coefficients and new pressure field to compute flux and then apply new velocity field to complete the equation)? 

September 21, 2015, 05:36 

#18 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 
the residual is computed for the discrete equation you really want to satisfy...if you linearized, this discrete equation must provide a vanishing residual. You cannot use the solution vector to compute the residual in a different discrete equation


September 21, 2015, 06:26 

#19  
New Member
Join Date: Jul 2015
Posts: 18
Rep Power: 9 
Quote:
And if one used deferred correction terms (eg bounded higher order schemes), are these computed for residuals or is it safe to ignore them? 

September 21, 2015, 06:44 

#20  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,290
Rep Power: 67 
Quote:
in the residual you must consider any discrete term you used in the computation... in symbolic term, said vn the solution at step n and A the discrete operators containing all fluxes (bounded or not), the residual at step n can be written (similar to interative methods for linear algebric systems) A(vn)  s = rn somehow, for steady solutions, rn can be interpreted as the time derivative you want to drive to zero 

Tags 
incompressible flow, parallel plates, simple 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Running parallel case after parallel meshing with snappyHexMesh?  Adam Persson  OpenFOAM Running, Solving & CFD  0  August 31, 2015 23:04 
radiation b/w parallel plates  str6073  FLUENT  0  November 18, 2013 08:42 
Injection between parallel plates, homogenous mode  Terje  CFX  7  September 7, 2008 20:51 
Flow between 2 parallel flat plates  pelli  FLUENT  2  July 14, 2007 10:59 
Parallel Computing Classes at San Diego Supercomputer Center Jan. 2022  Amitava Majumdar  Main CFD Forum  0  January 5, 1999 13:00 