
[Sponsors] 
September 29, 2011, 07:35 
Repeated table input

#1 
Member
Hamza Motiwala
Join Date: Nov 2010
Posts: 41
Rep Power: 8 
Sponsored Links
I am simulating an Exhaust gas recirculation model and I give in my input in the form of a table. The table is divided into 720 time steps corresponding to each crank angle turned. I want to repeat this cycle a couple of times. How can I get starccm+ to repeat the cycle everytime it reaches the end of the table. As a work around I had copy pasted the data one after the other 5 times in the same excel sheet along with increasing the time respectively to run the cycle 5 times . Is there a way to do it automatically? thanks, Hamza 

Sponsored Links 
October 1, 2011, 18:08 

#2 
Senior Member
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 14 
It is possible, but I have to check how to do it.


October 3, 2011, 05:12 

#3 
Member
Hamza Motiwala
Join Date: Nov 2010
Posts: 41
Rep Power: 8 
Thanks! I really appreciate it.


October 5, 2011, 19:08 

#4 
Senior Member
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 14 
Okay, the solution for your problem is:
 Read in the table for one cycle as usual. More than one cycle doesn't harm, but is not necessary.  Create a field function which uses the mod or fmod function (see field function programming reference in the online help) to give back a cyclic time. For example fmod($Time, 0.1) will take the current time and subtract 0.1 seconds until the remainder is less than 0.1. Let' call this $modTime  Create an interpolation field function. Interpolate the table (or the right column) by $modTime.  Use the later field function as input for your boundary condition Hope this helps 

October 6, 2011, 02:23 

#5 
Member
Hamza Motiwala
Join Date: Nov 2010
Posts: 41
Rep Power: 8 
Hey abdul,
Thanks for the reply. certain things are unclear to me. my timestep is .000060611 secs total physical time is .2181996 these are the field functions i wrote : modTime = fmod($Time, .000060611) interpolateTable(@Table("hd_egr"), "Time", SPLINE, "massflow", $modTime) now if my first time step would be .000060611 secs. I get a remainder 0 and then does the second field function above interpolate for a massflow value for time 0 in the table. If the remainder remains 0 all the time, how does it move further? I am lost here completely. I think I have not understood this thing correctly. How do I repeat the table n number of times? Can you explain further please? Thanks, Hamza 

October 6, 2011, 18:33 

#6  
Senior Member
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 14 
Quote:
modTime = fmod($Time, .2181996) So every time step your time will progress for 0.00006.... seconds until it finishes the first cycle. Then the cycle time will be cut and your simulation keeps on going, repeating the table from time the beginning. There is no number which defines how often the table should be repeated. The table will be repeated until your stopping criterias are satisfied and the simulation stops. So make sure your stopping criterias are set appropriate. 

October 7, 2011, 17:18 

#7 
Member
Hamza Motiwala
Join Date: Nov 2010
Posts: 41
Rep Power: 8 
Thanks a lot abdul!
I have made the necessary corrections and started the simulation. Hope to get some positive results on monday . 

October 12, 2011, 02:51 

#8 
Member
Hamza Motiwala
Join Date: Nov 2010
Posts: 41
Rep Power: 8 
It worked perfectly. Thanks a lot for the help man!


October 13, 2011, 17:00 

#9 
Senior Member
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 14 
You're welcome


December 7, 2011, 05:21 
exhaut converge

#10 
New Member
Join Date: Mar 2009
Location: Belgium
Posts: 13
Rep Power: 10 
Hi Hamza,
how do setup the physics conditions by Your calculation. My residuals is not really converge, I got Floiting Point exception after 3 cycles. Thanks, Rabat 

December 7, 2011, 09:51 

#11  
Member
Hamza Motiwala
Join Date: Nov 2010
Posts: 41
Rep Power: 8 
Quote:
I didnot understand your question. Do you want to know what physics models I used? I have run my simulations for as long as 14 cycles till now and I have had no problems. My first 2 or sometimes 3 cycles appear to be a little different from one another but later everything is fine. elaborate a little more and I will try providing more data from my side. Best Regards, Hamza 

December 8, 2011, 07:52 

#12 
New Member
Join Date: Mar 2009
Location: Belgium
Posts: 13
Rep Power: 10 
Hey Hamza,
which turbulant model did You use? I use at the moment: coupled energy, coupled flow, kepsilon turbulent and implicit unsteady. Did You change the solver parameters? Coupled implicit: courant number ramp or AMG linear solver How many inner iteration do you use? I would appreciate if You answer my quetions. Best Regards, Rabat 

December 9, 2011, 05:35 

#13  
Member
Hamza Motiwala
Join Date: Nov 2010
Posts: 41
Rep Power: 8 
Quote:
I have used both coupled and segregated models. currently I am simulating with Segregated and K Omega models. In my current simulation I have 40 inner iterations and I am running the simulation for 8 cycles that sums up to a total of around 230000 iterations. I did play with the courant number but since I am using segregated flow right now, its not relevant here. Apart from that I am using default values. No matter what the model, I think you should not have any problems running this code. You should be able to run it for as many cycles as possible. You should try running your simulation with default settings. What I dont understand is, if you can run the cycle once you should be able to run it a 100 times. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Input Parameter Value into Table  zephyrus17  CFX  0  February 9, 2011 23:22 
Fluent UDF: Thru external input  BS  FLUENT  0  March 26, 2008 19:53 
input curve BC  carno  Siemens  2  June 22, 2005 05:03 
Transient user input table  Bart  Siemens  0  January 10, 2005 02:27 
TABLE INPUT  LORENZO  Siemens  0  June 9, 2004 12:04 
Sponsored Links 