
[Sponsors] 
March 13, 2019, 06:21 
Initial pressure in water pipe flow

#1 
New Member
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 7 
Hello, my name is Ali. I'm a student and I'm doing a simulation with ANSYS 19.2 Academic about water flow in a pipe branch which has pump installed. I have velocity and pressure at the inlet (from experiment) and I used velocityinlet. I input the velocity about 0.6 m/s at 'velocity' and pressure about 86 kPa at 'supersonic/initial gauge pressure'. when I plot at a plane, the inlet I got is only about 100200 Pa gauge. I need the inlet pressure to be defined with that 86 kPa. how do I set its initial pressure since my flow is subsonic
I tried pressureinlet with 86 kPa but it turned out that the inlet velocity is far from 0.6 m/s. I need a suggestion about the inlet pressure I have or is there something I did wrong, thank you. reply if you need another details I simulated water flow in pipe branch and I used velocityinlet and outflow for 2 outlets. 

March 13, 2019, 07:16 

#2 
Senior Member
Moritz Kuhn
Join Date: Apr 2010
Location: Germany, Dresden
Posts: 207
Rep Power: 17 
The value supersonic/initial gauge pressure is only for supersonic flow which is not your case and for initializiation issues. Setting both, a pressure and a velocity at your inlet will be overdetermined. If you choose velocity inlet, fluent will calculate the pressure at your inlet as a result of the pressure drop in your pipe. The other way is, that you use pressure outlet and pressure inlet (means that you force the pressure drop of your pipe) and fluent will calculated the corrosponding flow velocity.
Choose pressure outlet, set the gauge pressure to 86 000 Pa, choose pressure inlet and set the gauge pressure to 86 150 Pa, and you will get something around 0.6 m/s 

March 13, 2019, 08:26 

#3  
New Member
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 7 
Quote:


March 13, 2019, 08:46 

#4 
Senior Member
Moritz Kuhn
Join Date: Apr 2010
Location: Germany, Dresden
Posts: 207
Rep Power: 17 
You can not use outflow and pressure inlet in one case. Choose velocity inlet and set the operating pressure ("Setting Up Physics" > "Operating Conditions" > "Operating Pressure") to 187325 Pa (default 101325 Pa + 86 kPa).


March 13, 2019, 10:36 

#5 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,682
Rep Power: 66 
You cannot fix the velocity and pressure at an inlet (unless it is supersonic). If you want to fix the inlet pressure, then use a pressure inlet and two pressure outlets w/ the targeted mass flow rate option. You should get something close to 0.6 m/s as the inlet velocity but it won't be exact. If you get something way off, then you made a mistake in your massflow input.


March 14, 2019, 03:11 

#6 
New Member
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 7 
Thank you LuckyTran & MKhun, I'll try your suggestion.
if I use a pressure outlet 0 Pa, does it means the pressure at outlet fixed at 0 Pa or ansys will calculate it? 

March 14, 2019, 04:49 

#7 
New Member
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 7 
Hello MKhun, I tried your suggestion I still get pressure about 200 Pa gauge. Any suggestion? thank you


March 14, 2019, 08:28 

#8 
Senior Member
Moritz Kuhn
Join Date: Apr 2010
Location: Germany, Dresden
Posts: 207
Rep Power: 17 
From your first post it is not clear if 86 kPa is your real set up the working pressure or the pressure drop. If pressure drop, than the value is realy high for a 0,6 m/s water flow, that means your pipe must be very long.
If you set pressure outlet to 0 Pa, then the absolute pressure at your outlet is the operating pressure (101325 Pa by default). Than you get 200 Pa at your inlet, the absolute pressure at your inelt is 101525 Pa, pressure drop over your pipe is 200 Pa. As water is an incompressible fluid, the pressure drop will be almost the same of 200 Pa, quite independent from your working pressure. So it doesn't matter if the operating pressure is 86 000 Pa, 101325 Pa or 187325 Pa. If you use pressure outlet and pressure inlet the pressue at these boundaries are almost fix. Fluent will calculate the resulting flow. 

March 15, 2019, 08:52 

#9  
New Member
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 7 
Quote:


March 15, 2019, 12:30 

#10  
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,682
Rep Power: 66 
Quote:
You've measured more things than you need to simulate the problem, which is good. But imagine you have measured the pressure everywhere and velocity everywhere? How do you apply these as constraints? The answer is, you don't! You have a choice how you want to model the problem because you measured more things than the minimum needed. But no matter what, you cannot apply everything that you measure as the constraint. For example, you can't force the velocity or pressure inside the pipe to be a certain value even if you measured it here. If you use a pressure outlet without using the targeted massflow rate option then the outlet pressure is fixed to the setting. If you turn on the targeted massflow rate setting, then the outlet pressure is still assigned to some value but it is slowly adjusted by Fluent each iteration so that eventually the outlet massflow matches what you put as the setting. 

March 18, 2019, 03:09 

#11 
Senior Member
Moritz Kuhn
Join Date: Apr 2010
Location: Germany, Dresden
Posts: 207
Rep Power: 17 
Set the operating pressure to 187325 Pa. Use pressure inlet with 101525 Pa. Calculate the mass flow at your outlet with the measured velocity. Than use pressure outlet with target mass flow rate. As already wrote be LuckyTran Fluent will calculate the pressure at the outlets.


Tags 
; pipe, initial condition, pressure and velocity, teejunction 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Problem with chtMultiregionFoam radiation boundary condition  baran_foam  OpenFOAM Running, Solving & CFD  10  December 17, 2019 17:36 
Segmentation fault when using reactingFOAM for Fluids  Tommy Floessner  OpenFOAM Running, Solving & CFD  4  April 22, 2018 12:30 
Extrusion with OpenFoam problem No. Iterations 0  Lord Kelvin  OpenFOAM Running, Solving & CFD  8  March 28, 2016 11:08 
simpleFoam error  "Floating point exception"  mbcx4jc2  OpenFOAM Running, Solving & CFD  12  August 4, 2015 02:20 
pisoFoam with kepsilon turb blows up  Some questions  Heroic  OpenFOAM Running, Solving & CFD  26  December 17, 2012 03:34 