
[Sponsors] 
displacemente pump as a momentum source in CFX 

LinkBack  Thread Tools  Search this Thread  Display Modes 
December 26, 2014, 11:09 
displacemente pump as a momentum source in CFX

#1 
New Member
ivan
Join Date: Dec 2014
Posts: 14
Rep Power: 9 
im new in CFD simulation in CFX. Im currently simulating a simple pipe system with one displacemente pump. i have read that with a "source" i can model the effect of a pump. i have issues with introducing the gneral momentum value. the system is simple
(in= 570 psi)=====PUMP====(out=2000 psi) i have done some runs (giving values to momentum) and have a flow to the output. in a simple way, how can i calculate the value of momentum or do a function to simulate the pump. i wanna a flow of 100 bpd to the output. from the pump i have a Q vs P table. thanks for advance 

December 27, 2014, 05:10 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,917
Rep Power: 132 
Put a pressure "sensor" at the inlet and outlet of the pump. This could be a probe point or a plane to do averaging over. You then have the pressure difference across the pump. Use the pump curve to give the flow velocity which would occur for this pressure difference and apply that flow velocity as a momentum source term (using the defined value approach  let me know if you are not aware of this approach).


December 27, 2014, 11:40 

#3 
New Member
ivan
Join Date: Dec 2014
Posts: 14
Rep Power: 9 
I really appreciate your response. I saw that the momentum is entered as c(v2v1) but i havent used this kind of approach. i have read too that i have to define a user function. i dont know if its necesary to use the p vs q of the pump cuz i already know that i have to keep a 100 bpd of flow and the diferencial pressure its going to be 2000 psi  570 psi. i dont know if iam taking this in the wrong way :S thanks for advance


December 27, 2014, 13:05 

#4 
New Member
ivan
Join Date: Dec 2014
Posts: 14
Rep Power: 9 
i have enter this in momentum source
(Velocity u  (0.0001840130728 [m^3 s1] /area()@in) ) but i dont know what to do next 

December 29, 2014, 12:44 

#5 
New Member
ivan
Join Date: Dec 2014
Posts: 14
Rep Power: 9 
im trying this in momentum source:
(massFlow()@in*(Velocity u  (0.0001840130728 [m^3 s^1] /area()@in) ))/volume()@Subdomain 1 

January 2, 2015, 17:11 

#6 
New Member
ivan
Join Date: Dec 2014
Posts: 14
Rep Power: 9 
i cant solve this problem =(, i really dont know how to implement C(v2v1) momentum source in this model. Any ideas?


January 3, 2015, 05:46 

#7 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,917
Rep Power: 132 
You seem to have made yourself very, very confused.
Have a look at section 1.3.2.2.2 General Momentum Source of the documentation (Modeling Guide) for how to implement this type of momentum source. 

January 3, 2015, 13:44 

#8 
New Member
ivan
Join Date: Dec 2014
Posts: 14
Rep Power: 9 
thanks for your reply. yes i read that. As far as i know i can model the pump effect like a momentum source, in CFX its a force/volume ok? thats why the unit are Newton/volume or kg m s^2 m^3. the way to do that it by the equation of Momentum Source s= C(v  vspec) in x y z components. where v is the variable of velocity, vspec is the one i specify (velocity that is function of the dp of the pump, in this case i want to keep it at 100 bpd that is an average velocity of 0.2 m/s in my case) and c as far i know is the coefficient of momentum that is the mass flow/volume , so i understand it as the mass flow that goes trought the pump and the volume of the pump giving units as kg s^1 m^3. but CFX modeling says that C is just a large number with units kg s^1 m^3 and that its good to define a coefficient to help convergence, so as far i cant understand i define it like
sx=100000 kg s^1 m^3 *(u  0.2 m s^1) sy= 0 cuz i dont want source in that direction sz= 0 cuz i dont want source in that direction coefficient= massflow enters the pump /volume of the pump whats your opinion, i messed all? ahaha sorry =( 

January 3, 2015, 23:35 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,917
Rep Power: 132 
You are close, but you missed the point of the coefficient. The equations are meant to be:
sx=C *(u  0.2 m s^1) sy= 0 cuz i dont want source in that direction sz= 0 cuz i dont want source in that direction C=100000 kg s^1 m^3 Momentum source term coefficient = C 

January 5, 2015, 10:37 

#10 
New Member
ivan
Join Date: Dec 2014
Posts: 14
Rep Power: 9 
thanks!!. So if i use the Mom Source Coeff. i define too like in the source entry? Is there a way to calculate that coeffcient intead of just "give" a large number?
thanks for advance 

January 5, 2015, 11:51 

#11 
New Member
ivan
Join Date: Dec 2014
Posts: 14
Rep Power: 9 
im trying this:
sx=100000000 [kg m^3 s^1]*(Velocity u  0.2 [m s^1]) sy= 0 cuz i dont want source in that direction sz= 0 cuz i dont want source in that direction C=1e+08 it take some time to convergence. im running in steady state, what do you think to run it in transient? i have seen i have trouble to convergence when the fluid start to go to the 2000 psi output as i increase C. it would be nice if i foud a way to calculate that number :S 

January 5, 2015, 17:10 

#12 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,917
Rep Power: 132 
You need the momentum source term coefficient to assist with convergence. Read the documentation about it.


Tags 
cfx, momentum, pumps, source 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
SparceImage v1.7.x Issue on MAC OS X  rcarmi  OpenFOAM Installation  4  August 14, 2014 07:42 
Problem compiling a custom Lagrangian library  brbbhatti  OpenFOAM Programming & Development  2  July 7, 2014 12:32 
OpenFOAM without MPI  kokizzu  OpenFOAM Installation  4  May 26, 2014 10:17 
Trouble compiling utilities using sourcebuilt OpenFOAM  Artur  OpenFOAM Programming & Development  14  October 29, 2013 11:59 
[swak4Foam] Error bulding swak4Foam  sfigato  OpenFOAM Community Contributions  18  August 22, 2013 13:41 