2D_simulation contd....
 

hi ,

i was playing with the timescale factor , increasing it stepwise to 2 , 4 , 6 , 10 , 20 and then checking how it affects the rate of convergence ,

1) i observed each time , there is an improvement in convergence rate , but this is remains for 20/30 iterations only

2) right from the outset my max. residual is 100 times corrspd. the rms values for all equations

3) after about 150 iterations, i notice a pocket of supersonic flow just past the obstacle - indicated by the red circle

4) i have noticed the flow 'recirculating' near the 'farfield' boundary - i have indicated this in the slide by the green circle

5)at 150 iterations ,there is 11% mass imbalance for the domain - flow coming 'in' from the 'farfield' boundary



doubts :

1) what could be the reason for the max. values being 100 times the rms values right from the start ?is it of concern ?

2) why the 'supersonic' pocket ? is it because my 'farfield' is too near at 1 m
from the obstacle ?

3) why the domain mass imbalance ?

if you could give some hints..

thanks & regards

sandeep

This FAQ explains a lot http://www.cfd-online.com/Wiki/Ansys...gence_criteria but maybe it does not explain much of the "why"...

2D_simulation contd....(update 16th _Jan
 

pl find attached the pictures showing :
streamlines
total pressure
global convergence
local convergence (monitor points at two locations)

i am getting a domain mass imbalance = 2. 3 % , and the residuals are also above 10^-5 criteria as shown in the slide

the total pressure i am getting is around 4 psi just upstream of the obstacle
whereas the calculations predict 18 psi (for upstream M = 0.6) , is this because of the 'farfield' being too close ?

should i take the 'farfield' boundary (bottom side) farther ?

pl give any hints as to how can i match the total pressure and get a good mass balance.

thanks

A detailed discussion is here: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

But in your case I can see a separation on the bottom wall/face which extends to the outlet. This is difficult to converge, so I would extend your outlet downstream so it is beyond any separation.

2D_simulation contd....
 

@glenn : the local convergence ,in this case ,appears good in the sense that the graph runs parallel -still i have tried to converge the continuity equation below 10^-5 ,but even when i do that , there seems to be no change in the locally monitored values , which are way off the analytically calculated values.

... gives me a feeling that moving the 'farfield' ('opening' at 1 atm.) further away might help to match the analytical values..am i right on this ?

I would just stay with an outlet but move it further downstream. Outlets are more numerically stable than openings, provided the flow is all in the same direction.

@glenn : firstly , sorry for this delayed update ...

1. the total pressure which i was reading from CFX was wrt 14.6psi Ref. Pr.
so, the absolute value of total pressure is 19.02 psi which is very close to 18.62 psi which i calculated using formula.

So, the values are not "way off the mark" as i felt earlier.

2. also there is no much qualitative (or quantitative) difference in the results when i increase the extent of the fluid domain - by moving the 'outlet' boundary further 2m downstream and i have interpreted the 'recirculation zone' near the 'opening' and 'outlet' boudaries as a SHEAR LAYER being formed when there is interaction b/w the moving air and the stagnant air as if present on the 'other' side of this 'opening' boundary.

Glenn i would like to know if you have any views on point no. 2 above ..the pictures are very much similar as the previous one which i had sent ..

thanks

Sandeep

If you are still getting a recirculation at the exit even after moving it 2m down stream then you have not moved it far enough. You need to move it far enough that the flow is all in one direction, with no reverse flow.