CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Initial pressure in water pipe flow

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 13, 2019, 07:21
Default Initial pressure in water pipe flow
  #1
New Member
 
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 5
mhmmdali is on a distinguished road
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 velocity-inlet. 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 100-200 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 pressure-inlet 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 velocity-inlet and outflow for 2 outlets.
mhmmdali is offline   Reply With Quote

Old   March 13, 2019, 08:16
Default
  #2
Senior Member
 
Moritz Kuhn
Join Date: Apr 2010
Location: Germany, Dresden
Posts: 163
Rep Power: 14
MKuhn is on a distinguished road
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
MKuhn is offline   Reply With Quote

Old   March 13, 2019, 09:26
Default
  #3
New Member
 
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 5
mhmmdali is on a distinguished road
Quote:
Originally Posted by MKuhn View Post
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
thank you for your answer. I'm doing my final project where I need to find the pressure at two branches and what if I change the outlet to outflow? since I have the data and I'm looking for outlet pressure based on flow split
mhmmdali is offline   Reply With Quote

Old   March 13, 2019, 09:46
Default
  #4
Senior Member
 
Moritz Kuhn
Join Date: Apr 2010
Location: Germany, Dresden
Posts: 163
Rep Power: 14
MKuhn is on a distinguished road
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).
MKuhn is offline   Reply With Quote

Old   March 13, 2019, 11:36
Default
  #5
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,112
Rep Power: 60
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
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.
LuckyTran is offline   Reply With Quote

Old   March 14, 2019, 04:11
Default
  #6
New Member
 
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 5
mhmmdali is on a distinguished road
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?
mhmmdali is offline   Reply With Quote

Old   March 14, 2019, 05:49
Default
  #7
New Member
 
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 5
mhmmdali is on a distinguished road
Quote:
Originally Posted by MKuhn View Post
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).
Hello MKhun, I tried your suggestion I still get pressure about 200 Pa gauge. Any suggestion? thank you
mhmmdali is offline   Reply With Quote

Old   March 14, 2019, 09:28
Default
  #8
Senior Member
 
Moritz Kuhn
Join Date: Apr 2010
Location: Germany, Dresden
Posts: 163
Rep Power: 14
MKuhn is on a distinguished road
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.
MKuhn is offline   Reply With Quote

Old   March 15, 2019, 09:52
Default
  #9
New Member
 
Muhammad Ali
Join Date: Mar 2019
Posts: 8
Rep Power: 5
mhmmdali is on a distinguished road
Quote:
Originally Posted by MKuhn View Post
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.
in my case, the inlet velocity is about 0.6 m/s (data taken using rotameter in a modul) and 86 kPa (data taken using pressure gauge) since I used a pump and split the flow into two branchs (90deg&180deg outlets). I'm trying to find the pressure outlet at those two branch and the data I have are pressure inlet, velocity inlet, velocity at two outlets. What is the best way to define my case? thank you sir
mhmmdali is offline   Reply With Quote

Old   March 15, 2019, 13:30
Default
  #10
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,112
Rep Power: 60
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by mhmmdali View Post
in my case, the inlet velocity is about 0.6 m/s (data taken using rotameter in a modul) and 86 kPa (data taken using pressure gauge) since I used a pump and split the flow into two branchs (90deg&180deg outlets). I'm trying to find the pressure outlet at those two branch and the data I have are pressure inlet, velocity inlet, velocity at two outlets. What is the best way to define my case? thank you sir

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.
LuckyTran is offline   Reply With Quote

Old   March 18, 2019, 04:09
Default
  #11
Senior Member
 
Moritz Kuhn
Join Date: Apr 2010
Location: Germany, Dresden
Posts: 163
Rep Power: 14
MKuhn is on a distinguished road
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.
MKuhn is offline   Reply With Quote

Reply

Tags
; pipe, initial condition, pressure and velocity, tee-junction

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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 18:36
Segmentation fault when using reactingFOAM for Fluids Tommy Floessner OpenFOAM Running, Solving & CFD 4 April 22, 2018 13:30
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM Running, Solving & CFD 8 March 28, 2016 12:08
simpleFoam error - "Floating point exception" mbcx4jc2 OpenFOAM Running, Solving & CFD 12 August 4, 2015 03:20
pisoFoam with k-epsilon turb blows up - Some questions Heroic OpenFOAM Running, Solving & CFD 26 December 17, 2012 04:34


All times are GMT -4. The time now is 10:17.