
[Sponsors] 
May 9, 2014, 13:34 
Periodic & Oscillatory Boundary Conditions

#1 
New Member
Emmanuel Kimuli
Join Date: May 2014
Posts: 5
Rep Power: 4 
Hi,
Am new to the CFD field and STAR CCM+ is the only software I have used so far. I am trying to simulate fluid flow in an Continuous Oscillatory Baffled Crsytallyser (COBC). I would like to have a net flow of about 0.002m/s and on top of that I would like to have an oscillatory flow. I have managed to set periodic boundary conditions for both the inlet and outlet of my fluid but I dont know how to super impose oscillatory flow onto the net flow. The oscillation velocity equation is 2π*f*x0*sin(2πft). where; f is the frequency (5hz), x0 is the amplitude and t is the time. Could someone please help me. Thank you in advance 

May 12, 2014, 07:29 

#2 
Senior Member
Ping
Join Date: Mar 2009
Posts: 257
Rep Power: 11 
where ever you have entered your net flow as a constant you can enter an equation of the flow as a function of time using the $Time field function  eg 3 * 1/5 *sin($Time) or whatever
so just recase your equation in those terms using the starccm+ field function equation syntax your could also create a user field function with the same equation and then use its name in place of the flow constant 

May 20, 2014, 05:56 

#3  
New Member
Emmanuel Kimuli
Join Date: May 2014
Posts: 5
Rep Power: 4 
Quote:
Thank you for your reply to my problem, I did as you advised me to i.e. At the inlet boundary conditions, for the velocity constant I entered; 0.002+(2*3.14*3*sin(2*3.14*5*$Time)) However the velocity magnitude doesn't seem to be changing with time, simply because the time isn't changing. I noticed this when i plotted velocity against time. I have attached the results in this reply, please have a look. Also while running the simulation, the output window shows that the software is solving at different time steps and it goes to a amximum of 1000, would changing the stopping criteria help improve my solution. I thank you for your help in advance. 

June 2, 2014, 03:50 

#4 
Senior Member
Ping
Join Date: Mar 2009
Posts: 257
Rep Power: 11 
the results you posted are all at the end of the run and so only show you the results at the last time which is at 1 second
I can see you have the implicit unsteady solver enabled and that the output shows the last two timesteps so you just need to create a few reports then monitor and plot these versus time and rerun the case eg i would create one of the surface average velocity magnitude on your inlet boundary and this will tell you if your velocity is changing the way you want it to you could also create a report of time in the region to convince yourself that time is actually changing 

June 3, 2014, 13:01 

#5  
New Member
Emmanuel Kimuli
Join Date: May 2014
Posts: 5
Rep Power: 4 
Quote:
Hello, I have managed to create a report, monitor and plot of surface averaged velocity magnitude at the inlet, it is constantly 0. I dont know why this simulation is coming out wrong. also looking at the contour and vector plots of the velocity magnitude on the plane i created along the pipe, the value is way lower that the one am expecting from the user field function i created; 0.002+(2*3.14*3*sin(2*3.14*5*$Time)). I should at least get a minimum velocit of 0.002m/s at any given time but am getting a highest velocity ~0.00001m/s. I set up periodic boundary conditions, by creating FullyDeveloped Interface at the inlet and outlet (Topology:Periodic). I then specified a mass flow rate of 3.92E5 kg/s at this Periodic interface. I have attached some results of my simulation and have tried to captue the simulation tree hopefully you can spot the mistake am making. 

June 3, 2014, 19:22 

#6 
Senior Member
Ping
Join Date: Mar 2009
Posts: 257
Rep Power: 11 
you were supposed to do the surface average velocity report etc on a boundary with flow ie in or out or an interface and not a wall where the velocity will always be zero when it has no slip enabled
i am confused about you boundary conditions since you talk about a constant flow of 3.92E5 kg/s somewhere but then also the equation with sin and $Time but you cant both try a simple velocity inlet with the equation and a pressure outlet and rid the interface when that works maybe try periodic with the equation as the mass flow remember when you create an interface the original boundary settings are ignored whether it be a wall or inlet etc 

July 4, 2014, 05:36 

#7  
New Member
Emmanuel Kimuli
Join Date: May 2014
Posts: 5
Rep Power: 4 
Quote:
Hi, I went ahead and removed the periodic interfaces, set the outlet boundary to a pressure outlet. then i used the field function i created as my velocity at the inlet. And I finally got the oscillating flow I was looking for, so yay and thanks to you. However my surface average velocity at the inlet doesn't seem to be what i was expecting (please find the files attached). the sine curve doesn't form properly and I don't know why. I would like to thank you very much for your help in advance and I hope to hear from you soon. I noticed my mistake, it was that I set up the report for surface averaged velocity magnitude instead of velocity in the xaxis direction. So please do not worry yourself with solving this issue. Last edited by R.B.Riddick; July 7, 2014 at 06:43. Reason: I noticed my mistake 

Tags 
boundary, cobc, conditions, oscillatory, periodic 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
ribbed channel / simpleFoam / boundary conditions  beeo  OpenFOAM PreProcessing  20  July 17, 2013 08:39 
Error finding variable "THERMX"  sunilpatil  CFX  8  April 26, 2013 07:00 
periodic boundary conditions fro pressure  Salem  Main CFD Forum  21  April 10, 2013 00:44 
Periodic boundary conditions in 3D Eulerian granular flow simulations  dsm  FLUENT  4  March 2, 2012 20:04 
periodic boundary conditions  mranji1  Main CFD Forum  4  August 24, 2009 23:45 